A: Yes. There are millions of parts in circulation; it is not possible to pre-package a library with all parts in it. There is a downloadable tutorial available for creating parts.

This link will download that PDF tutorial.
Procedure for getting maximum benefit from the Part Creation Tutorial:

1. The tutorial builds a part step-by-step. Build that part in PCB Artist along with the tutorial.

2. Refer to the overview of the PCB Symbol Wizard and Manual Part Creation in this document.

3. Note down any questions you have in the process.

4. Email the questions to layouthelp@4pcb.com when you have completed the tutorial.

Q: Can I get a quick overview of the Schematic Symbol Wizard?

A: Here is an overview:

Schematic Symbol Creation

Click on the Schematic Symbols tab in the upper left of the Library Manager.
Click on the New Lib button in the upper right. This will create a new Library for your part. Always put edited or created symbols of any kind in a library you created or you risk losing them in the future.
Click the Wizard button in the center column.

i. Click Next on the 1^st page

ii. Choose the Units and make the Precision 4 if you use Inches, Precision 3 if you use mm, and 1 if you use mils. Click Next.

iii. Choose one of the schematic shape symbols. In the upper right, change the Origin radio button to Pin1. Click Next

iv. On the Styles page, leave all at the defaults and click Next.

v. On the Pins page, distribute the pins on each side of the symbol as you wish. Leave the Distance between Pins, Width across Symbol, and Length Of Pin Leg all at the defaults. Click Next.

vi. On the Finish page, Name the symbol. Click on the Save Symbol to Library checkbox and change the dropdown to the library you created above. Click off the Edit Symbol New checkbox. Click Finish.

Q: Can I get a quick overview of the PCB Symbol Wizard?

A: Here is an overview:

1. Look up the data sheet of the part you need to create from the distributor or manufacturer.

a. Warning: If the data sheet shows a PCB footprint (which is rare), you should create to that footprint exactly as specified by the manufacturer.

b. Some types of specified footprints are easier to manually create (see below for manual part creation), than to create with the wizard.

c. Parts with no specified PCB footprint are usually easier to create in the PCB Symbol wizard.

2. Go to the Library Manager, which is on the top icon bar. It is the fifth icon from the left that resembles a book.

3. Click on the PCB Symbols Tab.

4. Click the Find button in the middle column. Search for the exact name you wish to call the part you will create. No two parts in the library can have the exact same name. Confirm the exact name is not used anywhere else.

· IMPORTANT - All parts you make or edit must be placed in a library of your own creation. They should never be placed in a library that came pre-packaged in PCB Artist. When upgrading PCB Artist, all of the pre-packaged libraries will be overwritten and new or modified parts residing in them. That directory can be backed up in advance of the upgrade, but the best practice to prevent data loss is to create your own libraries to store your new parts and also parts you have modified.

5. Click the New Lib Button on the upper right. This will create a new library and you will be asked to name it.

6. Click the Wizard button in the center column of buttons.

7. In the wizard Start page, click the Next button.

8. In the Technology page of the wizard:

a. You can choose to use a Technology file. Technology files save many types of settings from previous parts, such as Styles settings, Units settings, etc.

b. Units: This can be independently set from the schematic or layout units that you will use in your design. This should be set to the same units that the part’s data sheet.

c. Unit Precision: This controls how many decimal places are shown after the whole number of any displayed or entered numbers.

i. For example, if the Precision is set to zero and the Units are inches, a .250” hole would show as size zero.

ii. If the Units are set to millimeters and the Precision is set to 1, the user can enter a .25 grid to in Settings>Grids but the system will change it to .3.

d. Click the Next button.

9. On the Type page there are several packages to choose from. Choose SOIC for this example. Click the Next Tab.

10. On the Pads page you specify the dimensions of the part from off of the datasheet of the manufacturer.

a. A representation of the part is constructed on the right. It adjusts as you change values.

b. Notice that if you change the number of pads, the symbol changes on the right to match.

c. The gold and gray colored rectangle in the bottom center of the page:

i. Viewed from looking down upon it.

ii. The gold is the pcb surface mount land.

iii. The gray is the actual lead as it will sit on the surface mount land.

iv. The “H” dimension controls the heel, which in PCB Artist is defined as the sides and heel.

v. The “T” dimension controls the toe.

vi. The “PW” and “PL” dimensions represent the actual size of the surface mount.

d. Click Next to continue.

11. The Silkscreen Shape page is for specifying the details of the silkscreen. Click the Next Page.

12. The Placement Outline page is for specification of the part outline that will be placed on the Document layer. That layer can serve as an assembly drawing. Click the Next button.

13. The Finish page is where you save the part and specify its library. Make certain you are saving to a new library of your own creation.

Q: Can I get a quick overview of the Component Symbol Wizard?

A: Here is an overview:

1. Creating the Component. This will join the schematic and PCB Parts.

In the Library Manager, click the Component Symbols tab in the upper left.
Click on the New Lib button in the upper right. This will create a new Library for your part.
Click the Wizard button in the central column.

i. Click Next on the Start Page.

ii. Choose Normal Component and click Next.

iii. Details page:

1. Component Name will be the name of the symbol in the library.

2. Package is the type of package, you can type one in if you do not like the ones listed in the drop down menu. These names do not have any particular attributes that impact the part of its function.

3. Default Reference is the name the reference designator that will show on the silkscreen in the PCB layout.

4. Component Pins is as the name suggests. In selecting the part, it will only show PCB Symbols with this pad count in a particular library.

5. Number of Gates. For this type of part, just leave it at the default 1.

6. Click Next.

iv. Schematic Symbols page, first choose the library the Schematic Symbol was saved to, then select that part on the left. Make sure the Preview button is clicked on. Click Next.

v. PCB Symbol page works the same as the Schematic Symbols page. Make sure the Preview button is clicked on. Click Next.

vi. Assign Pins page, click the Assign 1 to 1 button. Click Next.

vii. Finish Page, choose the Component Symbol library you had created above. Make sure the Edit Symbol Now button is checked if you want to assign logic names to the pins, if you do not want that you must un-check this checkbox. Click Finish and the Component Symbol Editor will launch.

Manual Component Symbol editing.

The Gates column will be with only one gate, that is as is should be.
The SCH Symbol Name column should be left as is.
The SCH Symbol Terminal Name is where you can enter the logic names of the pins of the part. You do not have to enter them, but if you do not, they will not show on your schematic. On a BGA, it will likely be too crowded to display them.
The next three columns are for pin association. They should have the exact same number in each row.
The Net Class Name column should be empty.
Go to File Save. Exit the part.

Making the logic names show in the schematic.

Select the specific component, right-click and go to Properties.
Click on the Pin Names and Pin Numbers checkboxes to see those items.
Click OK to exit and save your change.
The logic names of a pad can be seen in the Status Bar in the lower left frame of the application without displaying them in the PCB Design.

Q: How do I create a connector or other manually created parts?

A: There are no connector templates in the PCB wizard. This is the process to create one. There are many other types of parts that are so different in footprint variation that they cannot have a common template in the PCB symbol wizard. These must be created manually.

1. Look up the data sheet of the part.

a. Warning: If the data sheet shows a PCB footprint (which is rare), you should adhere to that exact footprint in regards to hole sizes and any surface mount land patterns. Thru-hole pads should use a pad that has no less than .014” annular ring.

2. Most Data sheets use relative dimensions to define the part. We must manually convert all of these to absolute dimensions from of a point we can easily reference.

a. Print out the data sheet, it is recommended to blow up the dimensioned area. Use a pencil to make the conversions and note these absolute dimensions on the print-out as seen in the example below (the notes are in red).

b. Choose an easily accessible point on the part as the origin from which all absolute dimensions will reference. In the graphic example below, the indicated hole will serve as the origin and all manually converted absolute dimensions referencing it are in red.

c. You must always determine the x and y location of each mounting hole and also the lower left component hole of each grid of component holes.

3. Go to the Library Manager, which is on the top icon bar. It is the fifth icon from the left that resembles a book.

4. Click on the PCB Symbols Tab.

5. Click the New Lib Button on the upper right.

· All parts you make or edit must be placed in a library you have created.

· When upgrading PCB Artist, prepackaged libraries will be overwritten (unless they are backed up in advance). To prevent data loss, the best practice is to make new libraries.

6. Click on the New Item button. This opens an editing screen similar to the Edit PCB screen.

7. Making your pad and hole sizes.

a. Go to Settings>Units and set the units to the type used in the part drawing. In this example, use Inches with Precision set to no less than 3.

b. Go to Settings>Styles.

c. Click on the Pads Tab.

d. Making the Component Pads Style:

i. Click on the Add Style button

ii. Give the pad a name. This is its Style Name, which you should note down. For this example, call this CompPad1.

iii. Make Drill the finished hole size suggested by the manufacturers drawing. In this example .040”

iv. Make the pad (Width) no less than .014” (.36mm) over the hole size. In this example, the hole is .040” and the pad is going to be no less than .054”.

v. Click on OK to add the Style.

e. Creating the Mounting Holes Style:

i. Click on the Add Style button

ii. Give the mounting hole a name. This is its Style Name, which you should note down. For this example, call this MountingHole1.

iii. Make Drill the finished hole size suggested by the manufacturers drawing. In this example .096”

iv. Make the pad (Width) the same size as the mounting hole, .096” in this example. The pad exists as a presence on Top Copper for other features such as Pour Copper to avoid. In manufacturing, the pad will be removed.

v. Click off the Plated checkbox.

vi. Click OK to save and exit the dialog.

vii. A warning will say that the drill completely removes the pad.

viii. Click OK to save and exit the Styles dialog

8. Place the Mounting holes.

a. Placing the Origin.

i. Because the datum is a mounting hole, we must place them first. The origin position defaults to the first pad placed.

ii. Click Add Pad, drag the cursor to the work area, but do not add it yet.

iii. Click the <s> hotkey to choose the Style of pad to add. Choose the mounting hole you had made from the list.

iv. Add the pad.

v. Change to Select mode by clicking the white cursor arrow far right icon on the top icon bar. The icon looks like the cursor.

vi. Select the pad, right-click on it, and choose Origins>Set System Origin At Item (NOT “At Cursor”) from the right-click context menu.

1. All dimensions displayed or entered in the design are now based off the center of this pad.

b. Placing the second mounting hole.

i. Click Add Pad.

ii. The Style will be the same as the last one used, so it’s not necessary to change it.

iii. Place it anywhere.

iv. Change to Select mode by clicking the far right icon of the top icon bar. The icon looks like the cursor.

v. Select the pad that was just placed, right-click over it and go to Properties.

vi. In Properties, Type its destination X and Y axis coordinates in the Position fields. In this example, those coordinates are X=1.35, Y=0.

vii. Click OK. The mounting hole will move to those target coordinates.

9. Placing the grid of component pads.

a. Go to Settings>Grids. Click on the Working Grid Tab.

b. Change the first textbox of the Step Size section to the X axis coordinate of the lowest component pad in the far left. In this example, that is .525” (the true coordinate is -.525”, but the grid system does not accept negative numbers and a negative number is not necessary).

c. Click on the Different Y checkbox. In that blank type in the Y axis coordinate of the lowest component pad in the far left. In this example, it is .150” (the true coordinate is -.150”, but the grid system does not accept negative numbers and a negative number is not necessary).

d. Click OK to accept the changes and exit the Grid dialog.

e. Click on Add Pad. Drag your cursor to the work area, but do not place any pads.

f. Right Click and choose Add Multiple from the right-click context menu.

g. The Add Multiple dialog window:

i. In the Number of Items section, we must set how many pads we are adding in the X and Y.

1. In the X, we are setting 4 component pads (for this purpose, ignore the stagger on every other row). Set the X to 4

2. In the Y we are also using 4 in the Y axis. Set the Y to 4.

3. Many options on this screen that were grayed out are now editable.

ii. The Step Offset Section.

1. The X is the center-to-center distance between pads in the X axis. In this example, enter .150” in the X.

2. The Y in this example is .100”. Ignore the shift offset for now. In this example enter .100” in the Y.

iii. The Insert Order Section.

1. In this case, make sure the toggle is set to Insert Row. This is due to the fact that every other row is staggered. (If changed to Insert Column, then every other column would be staggered.)

2. Stagger Pitch is to establish how much the 2^nd row is staggered from the 1^st. If set to Insert Row, this is create a stagger (or indent) an X axis dimension. If set to Insert Column, it would be a stagger in the Y axis dimension. In this case the stagger is -.050” (the negative number is allowed and necessary). The negative number means the 2^nd row will start further to the left than the 1^st row. If the drawing showed the second row starting to the right, it would be a positive number (.050”). Enter -.050”.

iv. Click Ok to save your settings and exit that screen.

h. Click the <s> hotkey and choose the appropriate Style for this pad. In this example, use CompPad1.

i. Now move your cursor until it is at the correct position. Use the Status Bar coordinates in the lowest left frame of PCB Artist to ensure you are at the correct grid coordinates. Then click once to add that grid of component pads.

j. Add the second grid of component pads using the same process as described above, with these exceptions:

i. Go to Settings>Grids and change the grid X to .125” and leave the y as offset at .15.

ii. Change the number of items in X from 4 to 8.

k. Confirm the Dimensions are correct.

i. Find each dimensioned pad, right click on it and choose Properties from the right-click context menu. Confirm that the coordinates displayed in Properties are correct.

ii. Use Origins>Set System Origin At Item to change your origin to confirm that the part data sheets original relative coordinates are correct.

iii. Warning: Confirm every relative coordinate on the data sheet.

1. This verifies:

a. That the conversion to relative coordinates was done correctly.

b. That nothing was incorrectly typed in.

c. That no assumptions or oversights occurred during the entire process.

2. Be aware that occasionally a manufacturer’s data sheet is incorrect, and the numbers do not add up. At this point the part manufacturer would have to be contacted for the correct dimensions.

10. Legend Edits.

a. Go to Settings>Grids and change your grid to a .050” grid. Click off the Different Y checkbox and click OK to save the changes and exit the dialog.

b. Click on Add Shape Rectangle

c. Hit the <L> hotkey and change your layer to the Top Silkscreen (if it isn’t already on the Top Silkscreen).

d. Use Add>Shape Rectangle to add the legend outline of the part by clicking in the lower left to start the rectangle and double-clicking on the upper right corner.

11. Go to Add>Reference Origin and Click on any open area. The “+R” is a place holder for the part’s reference designator. The actual reference designator text “Conn” would be applied when editing the Component.

12. Adding the Placement Outline.

a. The Placement Outline is a box, often a bit bigger than the Legend outline.

b. Add it in the same manner as the Legend.

c. This outline will go on the Document1 layer (or the Document 2 layer in some cases)

d. The Document layers are usable for Assembly Drawing layers, and the outline can serve that purpose, or can be used for many other purposes.

13. Changing the Part Datum

a. Find Pin 1 on the part Data sheet. In this example, it is the pin in the upper left.

b. Select that corresponding pad on your part, right click on it and choose Origins>Set System Origin At Item. That pad is now the 0,0 center.

c. Select the “+S” symbol that is the Symbol Origin. You many need to use the <n> hotkey to cycle through the different objects at that location until it is selected.

d. Right click and choose Properties from the right-click context menu.

e. Change its Position to 0,0. The Symbol Origin must always be on Pin 1.

i. It is recommended to always put the System Origin on pin 1 so that the pads on the PCB Grid. This make it much easier to route tracks to the pads.

ii. Some believe that placing the System Origin at the middle of the PCB Symbol helps CPL file (component position file) generation. The System Origin has no affect on the determining the center of components. Placing the System Origin at the center will often cause all pads of the component to not be on the PCB grid.

14. Renumber Pins

a. Pins are automatically numbered as they are added, including mounting holes. So when we placed our mounting hole origin for this part, it became pin 1. We must change this.

i. To View the Pin Names more clearly, go to View>Colors. Click on the Other Items tab of the Colors Dialog box in the upper left. Click on the Pin Names Checkbox.

b. Go to Edit>Renumber Pins.

c. Click OK in the Renumber Pins dialog box to start numbering pins.

i. Notice that in the Status Bar on the lower right application frame is now in Renumber Pins mode.

ii. You will also notice in the Status Bar the “Next Number” box indicates the number 1. This is the number that next pad you click on will be changed to.

d. Click on pin 1.

e. Click on each pin, in sequential order, until all the pins are numbered.

f. Lastly click on each mounting hole, they also must have a pin number.

g. Hit the <esc> key to exit Renumber Pins mode.

15. Save the PCB Symbol to the Library you have created for it.

a. Make certain that you are using a unique name that is not used anywhere else in the library.

b. You must add this new symbol to a Component Symbol to add it to any design, regardless of whether it is being added to a schematic or a PCB design.

16. Component Creation

a. Any part that contains mounting holes cannot be created with the Component Symbol wizard.

b. Use the New Item button in the Library Manager’s Component tab to create any components with mounting holes.

Q: I cannot find the part I am looking for. Am I not looking in the right place?

A: The most effective search method is using this method:

From the main menu, go to File>Libraries.
Click on the Component Tab.
Use the Find button in the central row of buttons.

Next to the Name field, Change the drop down menu from Is Exactly to Contains.

It can also be very effective to search by pin number, unless the pin count is very small.

If you cannot find the part you are looking for in 5 minutes, you should just create it.

Almost any part can be created in 5-15 minutes in PCB Artist, especially with the PCB footprint wizard.
That new part can then be saved into a library you create and is organized in a way that best suits your preferences.

Q: How do you make mounting holes?

A: You can make them in two different ways:

1. The Quick way:

a. Use Add pad to place the pads.

b. Use <cntrl> to select all of the pads to be changed.

c. Right-click on any one of the pads and select Properties from the right-click context menu.

d. Change the Drill to the required finished hole size.

e. Change the Width (which is the pad width) to the same size as the drill.

f. Click off the Plated checkbox.

g. A warning will say the drill removes the pad, click OK.

h. This method will not give a Style name to these holes and will make it difficult to group select the all of them by the Style name. This technically puts them into the “Unnamed” Style group with many other shapes making them tedious to have to select by group in the future.

2. The Best Practices way:

a. Go to Settings>Styles.

b. Click on the Pads tab.

c. Click the Add Style button.

d. Enter a Name by which the new style will be referenced.

e. Enter the Drill Size.

f. Enter the Width (which refers to the pad width).

g. Click off the Plated checkbox.

h. Click the OK button to save and exit.

i. An error message will say the drill removes the pad, click OK.

j. Click Add Pad and drag your cursor over the work area, but do not yet add the pad.

k. Click the <s> hotkey (or right-click and choose Change Style).

l. In the dialog box that appears, choose the name of the style you created.

m. Add the Pad(s).

n. The advantage to creating a style is:

1. You only need to go to Settings>Styles to edit all the holes in the group at one time in the future.

2. You have the ability to select and display all items using the Style in the Goto tab of the Interaction Bar.

Q: How big should I make a finished hole size?

A: Always research the manufacture’s part and use what they recommend.

· In the event that the manufacturer provides no information and all other information sources are exhausted, the hole should be make at least .010” over the thickness of the lead. This is intended as a rule of thumb. The burden of research and verification that the rule applies to a particular design scenario is upon the designer.

Q: How big should I make the pad size?

A: The minimum requirement is a pad that is .014” over the hole size. So for a .020” hole, make at least .034”.

Q: Do I need to make Soldermask clearances?

A: Here is now the soldermask layer works:

Thru-hole pads are placed on layer [All] automatically. This means they have pads on all layers when added to or translated into a PCB. This includes an automatically generated soldermask clearance of exactly the needed size.
If you use the PCB Footprint wizard, it will automatically place surface mount devices on the [Top] layer. The [Top] layer automatically creates a clearance for the surface mount device on the Top Copper layer, the Top Soldermask layer, and the Top Solder Paste layers.
If you place a surface mount component on a PCB and use Flip to change it to the solderside, all [Top] values automatically become [Bottom] and all other relationships to layers are treated accordingly.
If you need a soldermask clearance that does not correspond to a specific pad, such as a large soldermask clearance over the whole component, use Add Shape. Use the <L> hotkey to change your working layer to the Top Soldermask. Draw the polygon and then select any segment of it, right-click and choose Properties from the right-click context menu. In Properties, click on the Filled checkbox.

Use the Layers tab of the Interaction Bar to display only the Top Solder Mask layer(s) to view the shapes.

Be aware that all objects on the soldermask are clearances in the soldermask and everything that is black in the soldermask layer will have the green soldermask covering.
WARNING: If you create a contact land with copper pour it will NOT have a soldermask clearance. Copper pour is not the correct tool to make contacts with. A solder mask clearance would have to be manually created using Add Shape Polygon to create the cleared area on the appropriate soldermask layer and then go into the polygon’s Properties to click on the Filled checkbox.
WARNING: If you Add Pad and then use Properties to make it a surface mount, it will be associated to the [All] layer, where all thru-hole pads live, and will be present on every layer. Surface mounts must be on layer [Top] or [Bottom]. The netlist will also believe the surface mounts have an electrical connection to the other surface mount counter parts on the other layers, were none exists, and will display the ratsnets and autoroute accordingly.

Q: How do I place pads dimensionally on my part?

A: This is the process:

Print out your data sheet for the part.
Data sheets usually have relative dimensions. We need to manually create absolute dimensions to an origin which can be easily referenced on the design. Manually convert all dimensions to their absolute dimensions from that origin. You can place a pad to serve as the origin and delete it later if necessary (but this will require the use of Edit>Renumber Pins to correct).
Right click on the datum and click Origins>Set System Origin At Item. The displayed coordinates and grid will now be snapped to that object.
Go to Settings>Styles of the objects that need to be placed dimensionally.
Click Add Pad, drag the cursor over the work area, and hit the <s> to choose the Style to be added. Place the objects anywhere in the work area.
Select each object, right-click and choose Properties from the right-click context menu. Type in their absolute coordinates. When you click OK to save your edit and exit Properties, the object will move to those coordinates.
When all items are placed, change your origin as necessary to confirm all relative and absolute coordinates.

Q: How can I verify that the Component Symbol I created is correct?

A: Use this method:

After creating your part create a blank schematic by clicking on File>New.
Bring up the Interaction Bar (use the <F9> key to bring it up and also to hide it).
Click on the Add Component tab of the interaction bar.
At the top of the Interaction Bar, select the library of the part you created.
Select the part you created and drag it to the blank schematic.
Go to Tools>Schematicß>PCB>Translate To PCB.
Watch for an error message. An error message indicates that something is wrong in the Component Symbol.

This method allows a new user to verify they have built their first few parts correctly without finding out there is a problem after the entire schematic is laid out with many components requiring corrections.

Schematic Creation

Q: How do I create a Multipage Schematic?

A: Here is the process:

If you use the templates in the Schema library, you can use the Ansi symbols as templates for schematic documentation.
You use as many schematic pages as the workspace will fit.
The key to this process is in the spacing of the Ansi Symbols. To get them print as individual schematics, the spacing must need adjusting until they print correctly.
This link leads to an example of 4 schematic sheets. This example schematic may need to have its spacing adjusted between the individual symbols to print properly on your specific printer.
We would always recommend first placing the templates, then adjusting the spacing between the symbols until they print each individual sheet correctly before placing any other symbols in the schematic.
Use off-page references to make connections between the schematics.

Q: How do I create off-page references?

A: This is the process:

Draw a connection off of a pin. Drag it a few grid points and double-click to terminate it there. The connection will turn red to indicate an un-terminated connection.
Select the connection, right-click and choose Change Net from the right-click context menu. Choose the net that you want it joined to.
The color of the connection should change to black to indicate the connection is no longer un-terminated.
Right click on the connection again and choose Display Net Name to verify the process was successful at a glance.

Q: Where can I find power and ground symbols for schematics?

A: They are located in the Schema component library.

Q: How do I change the values of capacitors, resistors, etc?

A: Use either a window selection or the <cntrl> button (in the same way you can use it to select specific files in Windows Explorer) to select all the specific components of that type to have the value changed. Then right click on any one of them and choose Properties. In the Properties window, click the Values tab. Select the value in the list and use the Edit button to change it. All the components will now have the new value.

Q: I made the symbol, but it doesn’t show on the list for Add Component. Why is that?

A: Schematic and PCB Symbols cannot be added to a board directly. They must be first joined into a Component Symbol. Only Component Symbols can be added to a PCB or Schematic.

Q: How do I display pin logic names on the schematic?

A: This is actually done at the component level.

Go to the Library Manager
Click on the Component tab.
Go to the correct library and select the part. Click the Edit button
Enter the logic name in the Terminal Name column (third column from the left).

Save and exit.
Open the schematic and then go to Tools>Update Component.
If the logic names are not displayed, right click on the component and choose Properties. Click on the check box for Pin Names.
If the Pin Names do not show, go to View>Colors. Click on the Other Items tab and click on the Pin Names checkbox if it is checked off. Click OK to save your changes and exit the Colors dialog box.

The New PCB Wizard

Q: Can I change the board size later?

A: Yes, you can delete it and completely redraw it in the PCB, but it must be created and finalized before placing an order.

Q: What does Unit Precision mean on the Board page of the New PCB Wizard?

A: Unit Precision is found in Settings>Units. Precision is how many decimal places any displayed coordinates round up to. If you have the Units set to Inches and the precision is set to zero, then the displayed size of a .250” hole will be 0”. Set Unit Precision appropriately for the units you have selected. Recommended Precision for Inches is Precision 4, for Millimeters is Precision 3 and for Mils is Precision 1.

Q: What is a Board Template?

A: When you create PCB Designs, you can save as a template. That will save the board with all its settings, components, board outline, and even tracks and copper pours. You can then use that saved template to start a new design with all those features built in for future designs. It can be used to save as little as unit settings or as much as whole designs. Be aware that if you save a template for a design, the entire design is saved, not just select features.

Q: I don’t know how many layers I need on the Layers page, what do I do?

A: It is easy to add layers after the New PCB Wizard, but when eliminating layers, you can only eliminate the last inner layers. So if you create a 10 layer board and find out that you only need 6, when you go to change the layer count you can only eliminate layers 9, 8, 7, and 6 (the Bottom Copper will become the new layer 6). This also changes the possible plane layers to 2, 3, 5, and 6, which may be a major conflict of some of those layers are already routed signal layers. So it is recommended to start out with a small number of layers and then once the layout has progressed to a point that the need for more layers is unavoidable, add the layers then from Settings>PCB Configuration.

Q: I need a split plane and a mixed plane inner layers, how do I specify that on the Layers page?

A: The plane layers are intended as pure planes. They should never be edited under any circumstance, even to draw a single track. On the layers page, leave them as signal layers and then when editing the PCB, use Pour Copper to draw split and mixed planes.

Q: On the Board Parameters page of the New PCB Wizard, I don’t know the minimum track width and space I need. How do I handle that?

A: The default is 10 mils, you can change it in the design, but you will have to go to Settings>PCB Wizard when you are in the PCB design and change this value on the Board Parameters page. The system will not allow you to submit the order if this number is not correct. It will prompt you if this value is different.

Q: On the Board Parameters Screen of the New PCB Wizard, I see the options for v-score and Tab rout, but they are grayed out. How can I select those?

A: Basic Design Requirement orders cannot have a v-score or tab route, due to overwhelming request of customers seeking the lowest possible cost. This includes orders with arrays. To get those options, select Expand Design Requirement on the Design Requirement Page of this wizard.

Q: What should I use the Special Requirements text box of the Additional Requirements page for?

A: It’s intended for any requirements that do not already have an option in the wizard and also for extra details of items you can select. Some Examples:

If the board is a flex design and requires a thinner final thickness not listed on the board thickness drop-down menu of the Board Parameters page (but was verified as possible for your design, through PCB Artist Technical Support), this would be the place to specify it. Special billing or shipping information can be noted here as well any special instructions. The board has countersinks, use this space to specify the counter sinks and to differentiate which holes are the countersinks. You can return to this page from Settings>PCB Configuration once you are in the design.

Q: On the Production page, must I enter a part number and revision?

A: Yes, we must have a way to reference the part for future orders. The software requires both of those blank be filled out before order placement.

Q: I want an array, how do I configure it?

A: See the Array section, below. That contains all instructions and examples.

Q: When I ran the New PCB Wizard, I chose some options I need to change. Do I have to start over?

A: Some options ran in the PCB Wizard can be changed long after PCB creation. This can be done from the main menu click on Settings>PCB Configuration to change some values.

Warning: Reducing the number of layers in this manner can eliminate nets. If layers must be eliminated, go to Output>Net Completion Report to get a report of the nets that are now incomplete. Then from the main menu, go to Tools>Optimize Nets to make the un-routed net connections appear. They can be manually or auto-routed from that point. After they are routed, it would be wise to go to Output>Net Completion again to confirm nothing was lost.

PCB Design Edit

Q: The plane layers are just a bunch of pads, what happened?

A: Go to View>Powerplane>Show to view pure plane layers. Mixed and Split planes are technically signal layers (using pour copper to make the planes), so those layers are viewed normally as any signal layers is.

Q: How big should I make via pads?

A: Make the via pad style 010” larger than the drill size. So for a .018” via hole, make the pad style width .028”. Make certain that you are using the Via style in Settings>Styles or the Design Rule Checks will not know they are intended as vias and will flag them as annular ring errors.

Q: I created plane layers and they don’t have thermal connections. What happened?

A: In the New PCB Wizard, either no net names were assigned to the planes or they were not spelled exactly the same as the net name (proper case is required as well).

To fix this, go to Settings>PCB Configuration in the PCB file and go to the Layers screen.
Use the drop down menus for assigning the planes to the correct nets to ensure that nothing is misspelled or has a different case.
Go to View>Powerplane>Show and view each plane to confirm they now have thermal connections.

Q: How can I change a component to the other side of the board?

A: Select the component, right-click on it and choose Flip.

Q: How do I display just the layers you want to see?

A: Bring up the Interaction Bar with <F9> and Click on the Layers tab at the very bottom of the Interaction Bar. Right-click over the list of layers and choose the All Layers Off option. Then click on just the layers you want to view.

Q: When I display the Properties of an object the size shows as zero, but that can’t be right.

A: Go to Settings>Units and change the Unit Precision to a larger number. Precision is how many decimal places any displayed coordinates round up to. If you have the Units set to Inches and the precision is set to zero, then the displayed size of a .250” hole will be 0”. Set Unit Precision appropriately for the units you have selected. Recommended Precision for Inches is Precision 4, for Millimeters is Precision 3 and for Mils is Precision 1.

Q: I can’t seem to draw at odd angles, is it possible to do that?

A: Yes

Click on the icon of the type of draw you wish to make (such as Add Track, Add Board Polygon, Add Shape Polygon, Add Track, Add Copper Pour Area Polygon , etc.).
Click to Add the draw and move your cursor to the work area.
Before starting the draw, right click to open the context menu.
Select Segment Mode>Free
Now lines can be added at any angle.
If moving shape segments, use the Free Rubberbanding option from the right-click context menu to allow the attached segments to take any angle.

Q: Can I make Mixed and Split Planes?

A: Yes, on outer layers, just use Pour Copper. On inners, DO NOT make the intended inner layers plane layers, keep them as signal layers. This can be modified while in the design from Settings>PCB Configuration on the Layers page of that wizard. You can then create split and mixed planes using Pour Copper just as it would be done on the outers. Never try to draw on a true plane layer, not even a single trace.

Q: How do I draw on a different layer?

A: Here is one way to do it.

Click on Add Track
Right-click and choose Track Layer OR hit the <L> hot key.
Click the box that says Apply To All Segments if want the whole track on the layer you are switching to.
Select the layer you wish to draw on in the dialog box that appears. It will automatically default to a layer other than the one you are on, so just hit return to accept it if you are on a double-sided board and you will be on the Bottom Side automatically.

Q: I have a net highlighted. How do I turn off the highlight?

A: The easiest way is from View>Highlight Net>Remove Highlight.

Q: Can I make draws with 45 degree angles to the bends in my traces?

A: Yes

Click on the icon of the type of draw you wish to make (such as Add Board Polygon, Add Shape Polygon, Add Track, Add Copper Pour Polygon, etc.).
Click to add the start of the shape.
Right Click to open the Context Menu while you are still in draw mode.
Select Segment Mode>Miter.
You can now draw at angles and the system will automatically put all junctions at 45 degrees.
It may help to change your draw mode to Free. See the question above regarding drawing at odd angles.

Q: How do I select all the segments of a trace at once?

A: Push and hold down the <shift> key, then select the trace. You can also select multiple whole traces by pushing and holding down the <cntrl> and <shift> keys.

Q: What is the significance of the pad colors?

A: On the default color settings:

Grey pads are present on all layers.

In Properties, they show as being on layer [All].
Surface mounts should not be grey. If they do, the component needs to be edited to change them from layer [All] to layer [Top] (NOT to be confused with layer Top Copper! An object on layer [Top] automatically has a soldermask clearance and solderpaste clearance generated. I will also flip all those to the [Bottom] layer if the Flip option is used on the component.

Dark Red pads (using the default color settins) are on Layer [Top] IF they are a slightly darker red than the Top Copper traces. If they are the same shade of red as the traces, then they are not on the [Top] layer, they are on Top Copper and will have no soldermask or solderpaste clearance. They must be changed to layer [Top] in Properties (see previous bullet point).
Dark Blue pads (using the default color settings) are on layer [Bottom]. They are slightly darker than the traces on the Bottom Copper Layer. The have all the other properties of objects on layer [Top], described above.
Yellow pads are vias created by the application when using the autorouter, moving a track segment to another layer, or other processes where the application places the hole automatically. They are present on layer [All], but are not associated with a component. Most commonly these are vias.

Q: I need to change a pad (or trace) size universally, is there a faster way that editing the properties on each one?

A: Yes, here is one of several ways to do this:

First determine the pad style used from the properties box.
Go to Settings>Styles.
The Styles window will open, click on the Pads tab.
The names of each pad style are listed. A new style can be created or an existing style can be edited from this window.
Be careful to be sure that the change will not affect more pads than you intended to affect.

Various combinations of selections and added styles can be used to accomplish different goals in selectively changing styles.
The Interaction Bar’s Goto tab can be used as a powerful tool when set to styles. Right clicking on the name of the style and choose Select All Find Items is another way to select all the items and to see them all selected before editing them either with Properties or through Settings>Styles as described above.

Q: How do I set up a Pour Copper area?

A: Here is the process:

Draw the bounding box polygon Using Add>Copper Pour Area.

· You can draw right over the rout and the poured copper it will clip itself back from the rout by the exact amount required (which is set in Settings>Spacings).

· The copper pour will clip itself back from all objects in the area that are not on the same net automatically (the spacing used is set in Settings>Spacings).

· In Settings>Spacings, the Shapes row governs the distance the copper is clipped back from the copper pour. The entire Shapes row must always be set to no less than .010”.

Click on the Selection Icon to exit draw mode (from the top icon bar, the last icon on the right that looks like your cursor).
Click on any one segment of the bounding box you just added.
Right-click and choose Pour Copper from the right-click context menu.
In the dialog box, choose the net it should be on. Leave that text field blank to have the copper pour unconnected from a net.
Click on the Thermal Pads checkbox to automatically add thermal pad connections.
Click on the checkbox to remove Isolated Areas at the bottom of that dialog window. Isolated areas will cause rats nests to show those areas as unconnected. Isolated areas will behave as an antenna on the finished board. Another option is to use the Highlight checkbox and connect those isolated islands with vias to their proper net.
IMPORTANT - The copper pour is applied once to the area it fills. If changes are made after the copper pour (such adding vias, mounting holes, or moving tracks) the copper pour will NOT adjust to this new change. To have the copper pour adjust to those changes, simply select the bounding box of the copper our, right click and click Pour Copper again. The Pour Copper dialog box will appear with the exact same settings of the previous pour. Click OK and the pour will be adjusted considering the changes made to the area.
IMPORTANT – The copper pour bounding box is not actually a copper object on the board, it will not intersect traces or end up in the actual board. Do not delete the bounding box.

Q: I created a copper pour area, but it’s not filled. Is that correct?

A: The edit is not yet complete. Here is how to complete it:

Select any line or arc of the copper pour boundary that you have drawn on the copper pour area and right click.
Select properties from the right click menu.
Select the Pour Copper Option
In the next window, select the nets the copper pour will be connected to.
IMPORTANT – once the net is selected, several checkbox options in the widow become active. To have thermal connections, the checkbox for Thermal Pads MUST be checked in this dialog box.

Q: I have added new holes and traces in an existing copper pour. They are not on the net of the copper pour, but they are connected to it. How do I fix this?

A: Select one segment of the bounding box, right-click and pour copper again. It will re-examine the connected tracks, holes, routs, etc and re-pour to clear back from them. Some notes on this:

All previous settings of the previous copper pour will be preserved in the dialog box. So if those do not need to be changed, just click the OK button to re-pour.
New isolated areas may be created by these new edits. If the Remove Isolated Areas check box is checked, these new isolated areas will be removed automatically.
If you DO NOT re-pour the copper, all those new edits will cause shorts to each of those individual nets.

A: No, the bounding box of the copper pour remains after the copper pour and does appear to intersect all traces it crosses. However it is not really present and is gone when the data is output. WARNING: Do not delete the copper pour’s bounding box in case you need to re-pour the copper again at a later stage.

Q: How close do I need to keep the copper pour from the rout edge?

A: You can draw the bounding box right over the rout edge and it the copper pour will automatically clip itself back from the rout to the exact amount necessary.

Q: I cannot select what I wish to select. Other items at the same point keep getting selected. How can I select the feature I want?

A: Use the “N” hotkey to cycle through objects at that location until the object you want is selected.

Q: How do I edit the soldermask?

A: That answer is above in the Component Creation section.

Be aware that all objects on the soldermask are clearances in the soldermask and everything that is black in the soldermask will have the green soldermask covering.

Q: How do I make mounting holes?

A: That answer is above in the Component Creation section.

Q: How do I create Slots?

A: Here are the procedures for making plated slots, non-plated slots, and slots for components.

Non-plated Slots can be made using the Add Board polygon. Any Board outline within the main board outline will be treated as a hole. The minimum width of any slot is .031”.
Plated Slots for PCB and PCB Symbols.

· This is a new feature for version 1.1.2 or later. If you have PCB Artist 1.1, go to Help>Check for Updates to download that patch. If you version is older than 1.1, download 1.1 from www.pcbartist.com.

1. Go to Settings>PCB Configuration in the design (or if you are making a component symbol, just make sure this step is done before adding the component or the plated slot will not appear in the component).

a. On the first page of that wizard, set the design to Expanded Service.

b. On the Board Parameters page, click on the checkbox for Plated Slots.

c. Go to the Production Page of the wizard and click the Finish button.

2. Go to Settings>Styles

a. Create an Oval pad style that is the exact dimensions of the finished plated slot.

· The Smallest width possible .026”

· Made the Drill Hole size zero.

· Give it a name, such as Slot

b. Create an Oval pad style that will be the pad of the plated slot.

· The width and length of the pad should be .014” over the slot dimensions at the minimum. (For example, a .030”x.150” slot must have a pad no smaller than .044”x.164”.)

· Slot pads Slots should always be on layer [All], which they will be on by default when built in this method.

· Make the Drill zero.

· Keep the Plated box checked.

· Give the style a name, such as SlotLand.

3. Click Add Pad. Move your cursor to the work area, but no not add anything yet.

4. Click the <s> hotkey and choose the style of the slot created in step a above (not the slot pad style created in step b).

5. Place the pad at its correct final dimensional location.

c. Warning – once the slot is changed from a pad to a draw, using copy and paste or move features will no longer be grabbing the object from center, but from the center point of the lines in the oval.

· This means the pad must be placed in the required position before conversion to a slot polygon.

· This also means that multiple slots placed with copy and paste should be completed at this point and not after conversion to the slot polygon.

6. Select the oval pad.

7. Right click on the Selected Oval Pad and choose Change Shape Type. In the drop down menu, choose Shape.

· Warning – Do not change origins or grids from this step until the slot land is added.

8. Click Add Pad. Move your cursor to the work area, but no not add anything yet.

9. Click the <s> hotkey and choose the style of the slot pad created in step 1-b above (not the slot style created in step a).

10. Add the pad right exactly over the center of the slot.

11. The Plated slot will be viewable on layer Plated Slot of a PCB Symbol and/or on layer V of the PCB Design.

Q: How do I put a radius or chamfer on my rout corner?

A: If you double click on 90 degree rout corner, it will take the corner into Miter or Fillet mode. In the Status bar in the lower left frame of the application, the phrase Edit Miter (or Fillet) Mode will appear. When you drag the cursor, it will increase the Fillet or Chamfer at each grid point. Go to Settings>Grids in advance of the edit to set the grid to the correct value. Right click while in miter (or fillet) mode to toggle between miter and fillet.

The Autorouter

Q: I have a fine pitch part that will not autoroute in the PCB. Why not?

A: There are a few different factors that constrain the autorouter with specific design rules. The key to successfully autorouting tighter pitched parts is in reducing the various rules the autorouter must obey:

1. Power and Ground tracks: Failing to route is often due to the trace width size being too large, especially power and ground tracks. The default power and ground sizes are quite large and can perhaps be much smaller, depending on the power requirements of the board.

A. The track size used by the autorouter is determined by the Net Class assigned to a net from Settings>Nets. Power Class and Ground Class will be routed with the Power Nom track style and Signal Class nets (the default class to any net) are routed with the Signal Nom track style.

B. To change the tracks sizes used, go to Settings>Styles from the main menu. Click on the Tracks Tab.

C. From their click the Tracks tab.

D. Click on the Power Nom track style. The default size is 50 mils, which will not be able to connect to a .5mm pitch smd.

E. The trace width can be changed there for the entire board including traces not yet added to the board.

F. IMPORTANT: Please be sure to properly calculate trace widths that will accommodate the power requirements of the PCB. This link will take you to the 4pcb.com trace width calculator. If the track size is made too small for the board’s power requirements, the track may become a fuse.

G. The autorouter will always use the Power Nom track style to draw the power traces unless the Minimum Width checkbox on the Autorouter checkbox is checked. In that case it uses Power Min. All other track styles are ignored by the autorouter.

H. Style settings can be saved (from a blank PCB file) from File>Save As Template if the sizes changed will frequently be used in other designs. (It is best to save templates from blank designs, so as not to accidentally save other features into the template, such as the board outline).

2. Signal Traces:

A. To change the traces sizes used, go to Settings>Styles from the main menu.

B. From their click the Tracks tab.

C. Click on the Signal Nom trace style.

o Track width can be set at small as 7 mil and be usable with Basic Design Requirement.

o With Expand Design Requirement, the traces can be as small as 5 mil.

o If a signal track width is changed from the default for either Design Requirement type, go to Settings>PCB Configuration. In the Board Parameters page of that wizard, change the Min Track Width/Gap to match the new smallest track on your design.

D. The trace width can be changed there for the entire board including traces not yet added to the board.

E. The autorouter uses the Signal Nom style from Settings>Styles in the Tracks tab to draw all signal tracks. If the Minimum Width checkbox is checked in the Autorouter dialog, it will instead use the Signal Min track style.

F. From their click the Tracks tab.

G. Style settings can be saved (from a blank PCB file) from File>Save As Template if the sizes changed will frequently be used in other designs.

3. Another factor in autorouting is the spacing requirements that the autorouter is constrained to follow.

A. If you go to Settings>Spacings, change the pad to track spacing.

o You can set the spacing to as low as 7 mils with Basic Design Requirement.

o You can set the spacing to as low as 5 mils with Expand Design Requirement.

o If a spacing is changed from the default, for either Design Requirement type, go to Settings>PCB Configuration. In the Board Parameters page of that wizard, change the Min Track Width/Gap to match the new smallest gap on your design (unless you already changed if for the track width, and it is the same number).

B. You can change whole rows or the entire grid by changing one cell, then clicking out of it, then right clicking over the cell you changed and choosing Apply to Row or one of the other options.

1. You can set the spacing to as low as 5 mils with Expand Design Requirement.

2. If you Apply to All, you need to change the Board row back to 20 and Apply it to the whole row. The minimum allowable is 10 mils for a tab rout or rectangular rout and 15 mil for v-scored designs.

C. Autorouter Grid:

1. In the Autorouter Dialog, a change to the Track Grid Size can free the autorouter to find new ways to connect.

2. The grid should be set to a derivative of primary grid. (For example, a 25 mil grid will not rout to a .5mm part. A 12.5 mil or 6.25 mil grid will allow the autorouter the freedom to do its job.)

D. Change Via Styles:

1. Got to Settings>Styles in the Pads tab.

2. Change the Via style to as low as .015” hole (with .025” pad) for Basic Design Requirement, as low as .008” (with .018” pad) for Expand Design Requirement.

3. If using Expanded Design Requirement and using a via smaller than .015 you must go to Settings>PCB Configuration and on the Board Parameters page of that wizard change the Minimum Hole drop-down to .010” (if you are using a pad smaller than .015” but larger or equal to .010”) or .008” if using a size smaller than .010”.

Q: How can I prevent the autorouter from drawing in a “keep out” area that I want it to avoid drawing in?

A: You can use Add>Shape>Rectangle or Polygon to block out an entire layer or area from autorouting. Draw the shape in the area you wish to exclude. Then select one segment of the shape, right-click and choose Properties. In the Properties dialog, click on the checkbox for Filled.

You can also use this method to create “Keep out” areas for the copper pour itself.
You should delete the filled shape after it has served its purpose.

Design Rule Checks

Q: Are there other checks to run besides Tools>Design Rule Checks?

A: Yes, under Tools>Schematicß>PCB use Consistency Check to verify the design when compared to your schematic.

Q: How can I review design rule check errors effectively?

A: Here are some effective ways:

Reviewing a small number of errors:

A. Select the error message itself.

B. Use the <n> hotkey to cycle between objects at that location until you have the error message selected.

C. Right-click and choose Properties from the context menu.

D. There should be a short message giving more information about the error.

Reviewing a large number of errors:

A. Bring up the Interaction Bar <F9>.

B. At the bottom of the Interaction Bar, click on the Goto tab.

C. At the top of the Interaction bar, change the drop-down menu to Error.

D. This will organize the errors by type and by layer. Click on the individual coordinate list to zoom to that specific error.

Q: I cannot get rid of all my design rule errors so I can investigate and edit them. How do I do that?

A: Go to Tools>Design Rule Check. In the Design Rule Check window, click the Delete Errors button.

Q: What do these Design Rule Check errors mean?

A: This is a very large and subjective question.

General Types of Errors:

Some design rule errors are per design and cannot be eliminated. The application is simply looking to bring something questionable to your attention.
Some errors are not un-manufacturable, but violate previously set design rules. For example, a design may have a 9 mil spacing error when the spacing is set for 10. The instance can either be edited to a 10 mil space or the Settings>Spacings screen can be edited to allow 9 mil spacing for that type of error.
Some errors are un-manufacturable or would produce a definite violation of IPC specifications.

The DRC Spacing checks are run according how Settings>Spacings is set. The grayed-out values cannot be changed. Other values can be changed, but may affect the pricing of the order.

All Spacings Design Rule Checks are measuring the distance from copper to copper with the exception of Board spacing and drill spacing.

It is important to remember that Text and Shapes are on an a copper layer are going to be copper and will have all the electrical properties of a trace or a copper pour.
Basic Design Requirement orders cannot have a track width or space below 7 mils. Expand Design Requirement orders cannot have a track width or space below 5 mils.
Spacing or Track width changes require the user to go to Settings>PCB Configuration and change the Minimum Track Width/Gap settings for the design on the Board Parameter page of that wizard. The application will not allow the order until that information is updated.
The Shapes row governs the distance the copper is clipped back from the copper pour. The entire Shapes row must always be set to .010” at the minimum.
Board spacing is for the distance between the board rout line to copper features.

Board to copper spacings should all be set at .020” as the default in Settings>Spacings.
For a routed or tab routed part, the settings could be set to .015” at the minimum
For a scored part, the minimum allowable spacing from copper is .020” or the designer risks exposed copper.

Drill spacing is to discover if drill holes are overlapping. This can happen when another hole is placed inside a much bigger hole by accident and cannot be easily viewable.

Most often this is seen when a via is accidentally placed inside another pad.
Click within the pad where you see the error and press <N> to cycle through objects present at the point the cursor was clicked on.
If the via is not totally within the hole, the yellow pad of the via may be visible.

Net Design Rules check for incomplete nets and also Dangling Traces.

Intentionally dangling tracks will produce an error message that will have to be ignored. Simply note the number of errors so when the order is submitted, you can see if the number of error has increased, indicating a new problem that must be investigated before ordering.

Add a Track to fix the error, if the connection is confirmed to be needed.
Use Tools>Optimize Nets (or the hotkey <cntrl> <d>) to have the software reconsider the netlist. Sometimes it will discover the connection to the net exists in a different path than it was expecting, elsewhere in the board.
If there was no schematic created, there is no way to verify the integrity of the design. A mistaken connection in the design can only be manually confirmed (if that).
Overlapping copper pour areas can cause this. The system is arranged so that overlapping polygons should never be necessary.
Isolated areas of a pour copper can cause this error. It is always best to re-pour the pour copper and click on the Remove Islands option. Isolated islands of copper behave as antennas.
Add Shape objects and filled polygons should only be used in areas too small for an effective copper pour. It is preferred to use copper pour wherever possible.
It is recommended to always ensure that the schematic is diligently preserved as the point of all changes (using Tools>PCBß>Schematic>Consistency check to forward differences from the schematic to the PCB), to avoid the most serious of these types of errors, even on the most simple board.

Manufacturing Design Rules cover many different areas of board design.

Minimum Line Width checks for tracks, draws and text using a smaller line .005”
Minimum annular ring check for:

.007” annular ring for component pads, minimum. That translates to .014” over the hole size.
.005” annular ring for via pads, minimum. That translates into .010” over the hole size.
Annular Ring Errors on mounting holes – The Plating checkbox in Properties has been left on. If it is clicked off, the errors will not continue to show.

Minimum Drill checks for holes smaller than .008”.
Text outside board test is to flag text that is outside of the PCB and may be an indication of an unplaced component.
Mirrored text check is to ensure that all solderside text is wrong-reading. Right-reading text on the solderside will be wrong reading after manufacture of the part.
Minimum solder paste test should be turned off and ignored. Solder stencil services vendors should have their own DFM tests that should perform for their customer depending on many factors that are unknowable.

· If there is doubt about the correct way to proceed, email your .pcb file and a brief description of your situation to layouthelp@4pcb.com.

Arrays

Q: What is an array (also referred to as a sub-panel, palette, etc)?

A: An array is putting multiple pieces of the same part number into frame to make small boards more manufacturable for fabrication and also to reduce assembly costs for small boards. To configure your design to be in an array, go to Settings>PCB Configuration and go to the Production Page of that wizard. Click on the Array Checkbox in the middle of the page to open the array options for editing. These are the various aspects of arrays:

The array size must be large enough to encompass all the individual pieces, the spacing between those parts, and the border material that holds them together.
The Borders are used for assembly operations to clamp onto securely without overlapping onto the board and interfering with assembly.
Tooling holes are also used for assembly operations to pin to. This is a more secure and precise way to hole onto the board than clamping to the borders alone.
Fiducials are used as optical targets for automated assembly. They are used to determine precise board alignment.
Scoring is a “v” grove cut into the top and bottom surfaces of an array configuration of multiple PCB’s or a PCB with removable rails or frame. The cut depth is set such that the material left is the lesser of .018” or 1/3 of the finished thickness. When this process is used the printed circuit boards are typically set up side by side and end to end with no gap between the edges. This results in the v-grove cutting into the area of the boards, so a .020” clearance between the edge of the boards and any conductors is required.

a. When placing an order that requires scoring please indicate this requirement by setting going to Settings>PCB Configuration.

b. On the first page of that wizard, make the board Expand Design Requirement.

c. On the Board Parameters page, click on the V-Score checkbox on the right.

Tab Routing for Arrays uses the router bit that cuts the board from the production panel to cut slots between the individual images, leaving behind small “tabs” of unrouted material to keep the array border and individual connected as one.

When placing an order that requires scoring please indicate this requirement by setting going to Settings>PCB Configuration.
On the first page of that wizard, make the board Expand Design Requirement.
On the Board Parameters page, click on the Tab Rout checkbox on the right.

Q: How do I make an array for a design?

A: Go to Settings>PCB Configuration. Go to the Production Page of that wizard. Click on the Array Checkbox in the middle of the page.

1. The optimum array size for efficient panel usage and lowest possible production cost is 10.8” x 7.8”. The goal is to come as close to that array size as possible without going over.

2. Here is an example of a PCB that is 3.5” x 2.2 to set up in an tab routed array:

· To Determine the Array Width for PCB Artist, simply add up the x-axis dimensions. For this board, the array width must be no less than 11.5”. Simply add up .4” + 3.5” + .1” + 3.5” + .1” + 3.5” + .4”.

· The formula for the Array Width is the same, but for the Y axis dimensions. This array width can be no less than 5.3”. That is .4” + 2.2” + .1” + 2.2” + .4”.

· Borders to use:

o The .4” border around the board is the minimum recommended for by assembly companies. .5” is often preferred by assemblers.

o A .2” border is the minimum manufacturable and cannot be changed, other than to increase it. Assembly will be very difficult as only .1” will remain of material. Tooling holes and fiducials cannot be added to this size.

o To Add Tooling Holes and/or Fiducials to the array, you must have a minimum of .4” border per side to the array.

· Warning: PCB Artist currently allows a minimum of a .1” minimum border to accommodate scored arrays and will allow an order of a tab rout with a .1” border. However, this is not possible to produce and will cause the board to go on hold pending customer authorization to increase to a .25” border (.2” at the minimum) and approval of any associated changes to the cost of the order.

3. Here is an example of a 3.5” x 2.2” board in a v-scored array:

· The array width on this example can be no less than 11.3”. That is .4” + 3.5” + 3.5” + 3.5” + .4”.

· The array height on this example can be no less than 5.2”. That is .4” + 2.2” + 2.2” + .4”.

· There is no space between scored parts.

· The .1” border is the minimum allowed cannot be changed, other than to make it larger.

4. Using the PCB Artist Array Dialog:

· This example is using the tab rout.

· Note that the Array Width and Array Height have the word “mils” at the end of each field, indicating this board is set to mils, and the units entered must be in mils, as seen in entering 11.5” as 11500.

· Array Width is 11.5” (or 11,500 mils) as calculated above.

· Array Height is 5.3” (or 5,300 mils) as calculated above.

· Array up is the total number of parts in the array. In this case 6.

· Note that the Quantity ordered is 18 parts. 18 individual parts which is 3 arrays.

o The Quantity is for the total number of part numbers, NOT the number of arrays. Arrays are never counted, only the individual parts which are contained in the arrays.

o The Quantity MUST be a multiple of the number of boards in the array. It would give an error if I made the quantity 17 or 19. However, it would accept 6, 12, 18, 24, etc.

· IMPORTANT – Basic Design Requirement orders are heavily discounted and do not include v-scoring or tab routing. To get v-scoring or tab routing of an array, you must go to Settings>PCB Configuration and set the board to Expand Design Requirement. Then go to the Board Parameters page of that wizard and click on the checkbox for either v-score or tab routing (or both).

Q: Cant I just Copy and Paste to create the array and skip the other way?

A: Yes, but it is not recommended.

The schematic will now not be able to verify the design
The silkscreen reference designators auto-number, meaning that R1 on one part will not be R23 on the second part pasted into the array and r41 on the next part pasted in. This will reflect on the BOM, but basically very problematic in production assembly.
It is possible that in selecting the part across several layers that something may be missed and not copied, which a schematic comparison will now be unable to catch.

Order Process Questions

Q: How do I place an order?

A: This link takes you to instructions to the ordering a Basic Design Requirement order.

This link leads to instructions to place an Expanded Design Requirement order.

Q: I clicked on Output>Submit order and it says that I have errors. What should I do?

A: The submit order process automatically runs the Design Rule Checks as part of Submit Order to prevent the possibility of not running them before ordering and also to catch accidental edits that the customer may not have been aware of.

If the Design Rule Checks have not been run, it is critical to check them before submitting the order.
If the checks have been run and the number of errors is verified as per design, click to ignore the errors and continue the order process.

Q: The order process is looking for a .fab file. What is that?

A: The .fab file is a copy of the .pcb file you were working in when you hit the Place Order or Get Quote button in the Submit Order process. It also serves as a “frozen” version of the exact file that was ordered. If your order has issues and you need to send an edited file, do you edit in the .pcb file and email the edited .pcb file to us. The .fab file will not be up to date and should only be used when ordering online.

Installation

Q: I am getting a windows warning saying "Due to a problem initializing a Microsoft OCX control the grid cannot be displayed. This option has not been turned off in Preferences."

A: This is a known issue with some revisions of a Windows file. The fix depends on your operating system. It is worth checking the date and version of the MSFLXGRD.OCX file on your system. There are several different varieties of this OCX file in the field, some of them quite different in size and date but showing the same version number.

Windows Vista:

Right click on Start/Accessories/Command Prompt and select Run As Administrator.
Type: CD C:\Windows\System32 <enter>
Type: regsvr32 msflxgrd.ocx <enter>
Type: exit <enter>
Right click on the PCB Artist program icon and select Run As Administrator.
From the PCB Artist main menu, go to File>Libraries
Go to the Components Tab, select any component from the left-hand list, and click the Edit button from the central list of buttons.
Exit without saving and Close the PCB Artist program.
Restart the PCB Artist normally.

The key point here is that the "Run As Administrator" option is only available from a menu or shortcut, so you need to launch the command prompt itself in this mode by finding it on the Start menu.

Windows XP/2000/ME/98/95:

From the Start menu, choose Run
Type CMD (or on Windows 95/98/ME, type COMMAND), and click OK.
Change directory to the folder containing your Windows system by typing: CD \WINDOWS\SYSTEM32 <enter>

On some systems your Windows files may be somewhere different, such as \WINNT.
Use the Windows Search feature to locate the file if necessary.

Type: REGSVR32 MSFLXGRD.OCX <enter>.
You should get a message telling you that the control has been registered.
If you get an error message when running regsvr32, perhaps suggesting that although the Flexgrid control is present but cannot be registered.

Download the file from this link:
The file is compressed, unzip it and put it the unzipped file in CD \WINDOWS\SYSTEM32.
Repeat the process starting at step 1, above.

Q: During Installation, I get an error that says “Setup Needs Next Disk” and “Please insert disk 1 that contains the file layout.bin”. It won’t install, what do I do?

A: This is an issue with Installshield. This link shows how to complete the installation.

Q: Why do I get an error during installation saying I don’t have permissions to access a file?

A: This is a very old Windows XP issue that has come up many times over the years.

v WARNING: Advanced Circuits recommends seeking the aid of or retaining the services of an experienced IT specialist to deal with this Windows issue. Customers performing this edit do so at their own risk. It is possible to cause irreparable harm to the computer and lose all files on the computer by performing any edits to the registry.

v Before Editing:

Backup – This is the process for backing up the registry prior to editing it.

Go to Run and type: Regedt32 <enter>
Click on File>Export
Save the file to a directory and make a note of its location.

Restore - If the computer needs to be restored to its previous settings before the edit:

A. Run Regedt32 as was done in step a, above.

B. Click on File>Import

C. Locate the file from Step c above.

If the computer will not boot up:

Press F8 while it is trying to boot.
Choose the option to restore the last known good configuration.

v The Edit:

1. Run regedt32.exe (It has to be regedt32 NOT regedit).

2. Select the window HKEY_LOCAL_MACHINE ON LOCAL MACHINE.

3. Select the SOFTWARE key.

4. Click SECURITY (or PERMISSIONS) from the menu bar (under the "Edit" menu).

5. Click PERMISSIONS.

6. From the Security section, highlight USERS.

7. Check the option FULL CONTROL.

8. Click APPLY.

9. Click the ADVANCED button.

10. Highlight USERS from the Permission Entries section.

11. Click VIEW/EDIT.

12. From the permissions section, uncheck the DELETE option from the Allow column.

13. Click OK.

14. Click APPLY before continuing to the next step.

15. Check the option RESET PERMISSIONS ON ALL CHILD OBJECTS AND ENABLE PROPAGATION OF INHERITABLE PERMISSIONS.

16. Click APPLY again.

17. Click YES at the security dialog warning box.

18. Click OK to the message about registry editor not being able to set permissions on some keys.

19. Click OK back at the access control settings for the SOFTWARE key.

20. Click OK back at the permissions for SOFTWARE dialog.

Q: I am having an installation problem that may be due to a proxy firewall. How can I deal with this?

A: Please send an email describing the issue to layouthelp@4pcb.com.

Q: I cannot find the directory where my design is stored. Where is it located?

A: There is a link to that directory in Start Menu>All Programs>Advanced Circuits>PCB Artist Data.

In Windows XP and Windows 2000 the directory path is: C:\Documents and Settings\All Users\Documents\PCB Artist. This directory structure allows PCB Artist files in that directory to be stored in a way that allows all users of that computer to open and access the file.
In Windows 98 the directory path is: C:\Program Files\Advanced Circuits\PCB Artist.
To make files accessible to only the user, in the save dialog box navigate to My Documents and save the files there. The files cannot be shared with all users from that directory.
PCB Artist will remember the last directory it saved a file to and will default to continue to save there as is typical in many Windows applications.

Q: Are other operating systems supported?

A: At this time only Windows systems from Windows 98 to Windows Vista are supported.

Some users are successfully using PCB Artist on the following operating systems with emulation software:

Macintosh using Parallels
Macintosh using Virtual PC
Ubuntu Linux using Wine

Assembly

Q: How do I optimize the design for Advanced Circuits Assembly Services?

A: If you right click on a component and choose Properties from the right-click context menu. Then click on the Values tab. From there you can enter values for the Manufacturer, Manufacturer Part Number, Distributor, and Distributor Part Number.

If Advanced Circuits is providing a turnkey service of ordering the parts for an order, this information will tremendously reduce the amount of time spent ordering the parts. This would eliminate a large amount of redundant communication with the customer.
If the customer is providing the kit for the assembly, these populated values will make it easier for the customer to have a comprehensive list of exactly what to order.
PCB Artist will create files that help to optimize the assembly process. These files are embedded in the board design and only available for Advanced Circuits Assembly.
Do not put via holes inside surface mount lands, unless there is a critical electrical reason.
Always click on the Thermals Pads checkbox in the copper pour dialog when pouring copper. Via holes can be directly connected to the plane and is a separate checkbox option.

Best Practices

v The file with the Tilde “~” in the front of it is the security backup. This is not your actual working file. The interval of how often it gets backed up is from Settings>PCB Configuration. If you set that to zero, it will not perform a backup, which is not recommended.

v Do not use Delete to remove tracks for redrawing.

1. Delete will remove the track and also its ratsnest connection. Delete is intended to completely remove the connection from the netlist.

2. To Remove the track, but not the connection:

· Select a segment of the track

· Right click on it and choose Nets>Unroute Track Segments (or Unroute Track Path) from the right-click context menu. The track will be replaced with an unrouted ratsnest connection.

v It is not recommended to use Undo to remove the results of the autorouter. Use Tools>Unrout Nets>All Nets.

v Be careful when joining nets.

1. A warning will appear such as this:

2. Be sure that the new net created by both is the correct one. This depends upon which net you were drawing with. Cancel and redraw your connect from the other net to make the resultant net the desired one.

3. Once the net is joined, it cannot be split. The smaller net must be deleted and redrawn.

v Avoid overlapping copper pours where possible.

1. Overlapping copper pours confuse the netlist.

2. If click down on the wheel of a wheel mouse, it will pan across the screen while dragging different types of draws including polygons. This makes drawing overlapping polygons unnecessary.

v Do not use copper pours for contact lands.

1. They will not have a soldermask clearance. They will be covered by soldermask, which is very hard to scrape off of the contact.

2. Options:

· Reconstruct them as surface mounts.

· Create a clearance of a filled rectangle or polygon on the soldermask layer.

v If your surface mount is colored gray, it requires a crucial edit.

1. Go into the Properties of the object and change them from layer [All] to layer [Top].

2. If the surface mount is part of a component, the edit must be done in the PCB Symbol editor.

3. This assumes that the default color settings are being used.

v Make sure your power and ground nets are properly defined in Settings>Nets as Power or Ground in the Class Column.

1. Power and ground traces usually need to be thicker than signal traces. All nets are classified as signal until the designer changes them to a Power or Ground Class.

v Plane layers cannot have draws or tracks on them.

1. They cannot have even one trace added to them.

2. If tracks must be drawn on them, change the layer to a Signal in Settings>PCB Configuration on the Layers page of that wizard and use Pour Copper to add the plane areas.

v Always create a new library for any parts you create or modify.

1. If a future version of PCB Artist needs a complete installation, any existing pre-packaged libraries are automatically overwritten and all parts will be lost.

2. All part creation documentation in this document describes the process of making a new library for your part.

v In Settings>Spacings, never change the Board row to less than .020” or the Shape row to less than .010”.

1. Those settings are not only for Design Rule Checks, but also provide rules for how copper pours are created.

v Do not create parts with the same name as any other part in any other library.

1. The system acquires parts in a hierarchy of libraries that are searched when symbols are updated in the PCB or Schematic. If the other part with same name in the other library are located first, it will now be associated to that symbol.

v Do not add Vias inside Surface Mount Lands.

Many designers add vias inside surface mount lands as a way of conserving space in a design. This creates greater difficulty and lower quality solder joints in assembly. This practice is not recommended unless absolutely necessary for electrical purposes.

v Always use Thermal Pads in Copper Pours for component holes.

Regardless of heat sink needs, always use thermal pads in copper pours for component pads. Thermals pads are not necessary on vias. Directly connecting lands to the planes will cause assembly problems are poor quality solder joints.

v Preventing accidental edits.

1. Making layers or object types unselectable is possible from View>Colors. Go to the Layered Items tab.

· The Selectable row locks objects by changing the cell from Yes to No with a double click of the mouse button.

· The Selectable column locks objects for specific layers by double clicking the cell from Yes to No.

· Individual objects can be locked from editing by selecting that object, right-clicking on it, and choosing Fix Item. This will prompt a dialog box asking for confirmation if an edit is attempted on a specific object.

If you have a new question, please don’t hesitate to send it to Layouthelp@4pcb.com