Frequently
Asked Questions
This page is not intended to replace the Design Tutorial in PCB Artist,
but to clarify important items for users.
The Design Tutorial is found in the PCB Artist application itself. It is accessible from the main menu under Help>Design
Tutorial.
More information is available
in the User Tips Guide for PCB Artist, which can be downloaded from this link:
Email technical support is
available at layouthelp@4pcb.com
Not finding the part you are looking for
The most effective search method is using this
method:
PCB Artist has an online
library available. This may be found: Here
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.
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.
Overview of the Schematic
Symbol Wizard
i.
Click Next on the 1st 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.
Overview of the PCB Symbol
Wizard
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.
Overview of the Component
Symbol Wizard
1.
Creating the Component. This will
join the schematic and PCB Parts.
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.
Manually
create a connector or part (simple)
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 Pad1.
iii.
If no hole size is suggested, it is recommended
that you make the hole .010” larger than the pin diameter. Since the diagonal
of the square is given, we will use that dimension as the diameter. In this
example, the four outer pins .060”, so the hole size needs to be .070”.
iv.
Make the pad (Width) no less than .014” (.36mm)
over the hole size. In this example, the hole is .070” and the pad is
going to be no less than .084”.
v.
Click on OK to add the 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 Pad2.
iii.
For this example, the pin size is .050”, so the
hole size should be .060”.
iv.
Make the pad width at least .074” for this pin.
v.
Click OK to add the style.
i.
Go to Add>Pad, but before clicking to add, type
the <S> key to select the style, (Pad1), then select OK.
ii.
Then, right click and select Add Multiple Items.
Since the four pads are symmetrically spaced apart, we can input the proper X
and Y distances from the centers of the pad. For this example they are spaced
.200” from center to center per the fabrication drawing.
iii.
Place the pads in the design space. Type the
<Esc> key to exit out of the Add Pad command. You can zoom in or out to
adjust for a proper view of the pad.
i.
Right click on the lower left pad and select
Origins>Set System Origin at Item.
ii.
Now, we need to set the grid up so that it will be
easy to place the center pad in the correct place.
1. Go to
Settings>Grids.
2. Set up
the grid so that it is at 50mil intervals and click OK.
i.
Since the grid is setup so that the center pad ill
be placed directly in the center of the four outer pads, go to Add>Pad.
ii.
Before placing, type the <S> key and choose
the center pad style (Pad2). Then place it in the center of the four pads and
type the <Esc> key so that you will not continue to add any more pads.
Manually create a connector or part (complex)
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 2nd
row is staggered from the 1st.
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 2nd row will start further to the left than the 1st
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 “
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.
Creating Gold Fingers and Edge connectors
Gold edge connectors have to be created as a component, similar
to a connector. This is a three step
process. First make the schematic
symbol, then the PCB Symbol, then join the two and associate their pins in
creating a Component. On the
instructions below, I am assuming you’re familiar with Part Creation Tutorial
and the Frequently Asked Questions document
of the PCB Artist Tips & Tools web
page.
Verifying a component symbol
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.
Pad size
The minimum requirement is a pad that is .014” over
the hole size. So for a .020” hole, make
at least .034”. For vias, the minimum
required pad is .01” over the hole size.
Mounting holes
You can make them in two different ways:
1.
The Quick way:
a.
Use Add pad to place the pads.
b.
Use <Ctrl> 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.
Make sure the mounting hole pad width is the same size as the
through hole.
Place pads dimensionally
Soldermask clearances
Here is now the soldermask layer works:
Non Plated Cut outs
in a Component Footprint
If a
component requires non plated cut outs within a component footprint, they will
need to be placed after the component is placed on the board. For reference one may draw the component
information out on the silk or documentation layer, but the same information
will need to be drawn on the Board layer.
Often a
component will need to be changed or updated.
Even if the component is updated just by the footprint, it should be
updated on the schematic and the PCB file to make sure the boards are
consistent. The function to update
components is found in Tools>Update Components>Browse. Although the option to update all components
is available, it is suggested to only update the one component selected through
the browse list.
Package
in component generation relates to the type of chipset and shape the component
part is. When creating a part, by
default the package is “User”.
The
following is a list of a few packages and possible footprints (details and
drawings are approximate, and are just examples):
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
Extracting
components from the .pcb and .sch files
One can
extract the components from a .pcb file and .sch file in the Library
Manager. To do so, go to the Library
Manager and select a tab. For the
schematic symbol, you will need the schematic.
For the PCB symbol one will need the PCB File. For a complete component (PCB And Schematic
symbols both) you will need both the schematic and PCB file found within the
same place.
Power and
ground symbols
They are located in the Schema component library.
Use either a window selection or the <Ctrl>
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.
Symbol doesn’t show on Add
Component list
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.
This is actually done at the component level.
Forward Changes from schematic to
PCB
Often when changes are needed on
existing board files it is best to do them to the schematic first, then forward
those changes to the pcb drawing. This
allows the schematic and pcb drawing to remain consistent, and for the designer
to run a consistency check to make sure both designs are still the same. To forward changes from the schematic go to
Tools>SchematicóPCB>Forward Design changes.
This will create a report that will state all the changes that has been
done to the pcb file. Forwarding Design
changes will unroute any nets that no longer match the schematic, remove parts
that are no longer in the design, add parts, and change net names.
You can
delete it and completely redraw it in the PCB, but it must be created and
finalized before placing an order.
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.
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.
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.
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.
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.
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 Expanded Design
Requirement on the Design Requirement Page of this wizard.
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.
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.
See the Array section, below. That contains all instructions and examples.
Change options after New PCB Wizard
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.
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.
Use the “N” hotkey to cycle through objects at that
location until the object you want is selected.
The easiest way is from View>Highlight
Net>Remove Highlight.
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.
Properties of an object display size as zero
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.
Select all the segments of a trace at once
Push and hold down the <shift> key, then
select the trace. You can also select
multiple whole traces by pushing and holding down the <ctrl> and
<shift> keys.
On the default color settings:
The
following information relates to what layers the feature will appear on,
function, or error.
|
PCB Color Coding: |
|
|
Gray: Appears on all layers, and the soldermask
layers. In the properties drop down it
will show as [All]. |
|
|
Red: Appears on the top copper only, and not the
soldermask. If this is a pad, in the
properties drop down it will show as [Top Copper]. |
|
|
Dark Red: Appears on the top copper and the top
soldermask. In the Properties drop
down, it will show as [Top]. |
|
|
Cyan/Teal: Appears on the bottom layer with no
soldermask clearance. If a pad, this
will show as [Bottom Copper] in the properties drop down. |
|
|
Dark Cyan/Teal: Bottom copper with
soldermask clearance. In the
properties drop down, this will show as [Bottom]. |
|
|
Yellow Pads: These represent vias. Vias appear on all layers. |
|
|
Bright Green: Board layer. The board layer is the outline/route of the
board. |
|
|
Dark Green: Documentation 1 layer |
|
|
Dark Blue: Documentation 2 layer |
|
|
Slate Blue: Top Silk Screen |
|
|
Purple: Bottom Silk Screen |
|
|
Orange/Coral: Top soldermask layer |
|
|
Light Gray: Bottom Soldermask layer |
|
|
Function colors: |
|
|
Thin yellow Lines:
Thin yellow lines indicate disconnected nets that may need to be drawn. These are commonly known as “Rats Nests”. |
|
|
Dark Blue Tracks/Pads:
This may indicate that a net has been highlighted. |
|
|
White: This is an actively selected object. |
|
|
Track with a Pink Inner Line:
This indicates a disconnected track |
|
|
Green Highlight: Non net highlight. One may turn off the highlight by going to
View>Goto>Remove Highlight |
|
|
|
|
|
Schematic Color coding: |
|
|
|
|
|
Cyan: Net Selected Connection Highlight |
|
|
Black: Un-highlighted
Connection/Schematic Symbol |
|
|
Pink: This indicates an incomplete
connection. |
|
|
Dark Cyan/Teal: Pin number |
|
|
Olive: Pin name, sometimes will show as
a N# as a designator |
|
|
Blue: Text, Symbol Text, and Value
Position |
|
|
|
|
Here is one way to do it.
Moving component to the other side of the board
Select the component, right-click on it and choose
Flip. This may also be done by selecting
the component and using the “F” hotkey.
It’s best not to have track connections to the component before placing
it on the opposing side.
Corners with radius or chamfer
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.
Make
draws with 45 degree angles
Often a track has to be partially redrawn if
clicking and dragging the track is not sufficient. To remove one segment of a track:
1.
Select the track, and right click on it.
2. Select
Net>Unroute Track Segments
The highlighted track segment will disappear. PCB Artist will consider both sides of the
track gap and all included pads and copper features to be still part of the
same net. This will be indicated by a
yellow line by default, commonly known as a “Rats Nest”.
Change a pad (or trace) size universally
Here is one of several ways to do this:
·
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.
Initially
PCB Artist is set up to not allow multiple tracks to connect the same two
points on a board. This can be bypassed
by going to Settings>Preference>Interaction tab, and putting a Check in
the box beside “Allow Duplicate Tracks”.
That answer is above in the Component Creation
section found here: Mounting holes.
Here are the procedures for making plated slots,
non-plated slots, and slots for components.
·
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
1.4 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” for an Expanded
board, .02” for a Premium Expanded.
·
Make 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 the
Plated Slot layer in PCB Artist.
a.
Warning – If a component with a plated
slot is placed before the option has been activated in Settings>PCB
Config>Board Parameters, the plated slots information that will show on the
plated slots layer will be lost!
Creating a complex
board Shape
The first
approach is if you already have a complex board shape created in .dxf
format. Then all that is needed is to
import the .dxf onto the Board layer.
See “How to
Import a .Dxf” for instructions.
If this
is not an option, then starting with a general board shape, then modifying it
will be your best option. Some of the most
complex board outlines may only be 5 or 6 continuous lines:
The above
outline started with a large rectangle Shape from
Add>Board>Rectangle. By double
clicking the board outline to modify segment (also an option available with
right clicking and selecting modify segment), we were able to pull and drag our
outline to a closer shape of the desired board. To deactivate the edit, double click
again. To reset the edit while editing,
one may hit escape and all changed features in the current edit will snap back
to the previous shape. It’s good
practice to have the grid (and Grid Snap) set to a desirable distance for
snapping to. The Grid snap and Grid
functions are available in Settings>Grids (or Ctrl+G). Segments may be changed into Arcs by right clicking
on a line segment and selecting Arc.
There will be various options there for different Arc degrees, and the
ability to also Flip the Arc.
Non
plated cut outs are created on the board layer with the board outline. One may go to Add>Board and select a shape. The smallest non plated cut out dimension
available is .031” on a Basic or Normal Expanded spec board. For a premium Expanded spec board, the
smallest non plate cut out dimension is .02”.
That answer is above in the Component Creation
section.
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.
Adding personal logos and symbols
to the Silk Screen or Copper layer
To add
personal logos into PCB Artist, we recommend creating the logo in a font editor
as a new Font. There are many font
editors available online. Once the logo
has been created in the editor and connected to a particular keyboard key, save
the file as a True Type Font with a distinct name. Install the font onto your system, but keep
it handy as it will need to be sent to Advance Circuits to allow processing of
your PCB Files. To place the logo into
PCB Artist, one will place it as a text using the newly created font with the
logo. Be sure to send PCB Artist the
true type font file. Make sure the true
type font’s name is very specific to avoid possibly overwriting the fonts in
our database and the possibility of your own personal font from being overwritten.
Long delay when
moving components on the PCB
The software is also capable of performing a
dynamic optimize during component move. When moving a component, right-click
and select the Place option from the context menu. Then move the component again
and right-click and choose Dynamic Optimize. This will remain a default choice
for all parts moved on all future designs, until deactivated. To
deactivate it, one may do the same option as above, and uncheck Dynamic
Optimize.
The most
common net classes in PCB Artist is signal, power and ground. These classes reflect not only the track
types and widths, but will reflect the type of vias added the connections. Net classes may be used to control the
defaults for track widths. To create a
new net class one may go to the Settings> Net Classes and click the “Add”
button.
In the
Net Class pop up, there will be options to set the minimum and maximum widths
of the tracks for this class, and options on how the vias will be set up. Once created the new net class can be
assigned to a net, and the net will reflect the properties of that new class
type. More one Net Classes will be found
in Help>Context Help, under Net Classes.
·
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”.
The edit is not yet complete. Here is how to complete it:
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.
Adding items in an existing copper pour
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:
Copper pour around the rout edge
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.
Thermal connections on plane layers
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).
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.
Currently,
PCB Artist may import .dxf files for mechanical functions (like outlines and
references) and OrCAD EDIF format netlists in place of using a schematic. PCB Artist is able to export .dxf format, and
allow printing to .pdf format (See Create a .pdf File). One will be able to export all layers but the
copper circuit, in .dxf format. Gerber
files are generated by request of the customer on boards that have been ordered
and processed by the Advanced Circuits CAM department.
How to import a DXF format file
One may
import a dxf format file into PCB Artist, using the File>Import
function. A pop up will give options for
import.
Instead
of using a schematic generated in PCB Artist.
There is an option to use an OrCAD EDIF format netlist instead. The option to do this is through
File>Import. Before doing this one
must have all the components already build into PCB Artist. One must also be aware of all the component
names found within PCB Artist and the OrCAD drawing. When importing the netlist into a fresh PCB
Drawing, The designer will need to “Edit
Map”. This pop up will initially be all
blank values. These value are manually
input to create an OrCAD.map file that PCB Artist will use as reference to
match the netlist in parts and net connections.
More about Importing OrCAD EDIF netlist may be found in Help>Context
Help under OrCAD Import.
To update
any changes done to an OrCAD EDIF netlist into PCB Artist one must use the ECO
From Netlist function. This is available
in File>ECO From Netlist, and requires the updated OrCAD EDIF netlist. Like Importing an OrCAD EDIF netlist, if any
new parts have been added, the parts will also need to be creating in PCB
Artist, and the OrCAD.map file will need to be updated. More about ECO from Netlist may be found in
Help>Context Help under ECO from Netlist.
Auto route with fine pitch components
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 Expanded 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 may 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
One may set the spacing to as low as 7 mils with Basic
Design Requirement.
o
One may set the spacing to as low as 5 mils with Expanded
Design Requirement.
o
One may set the spacing to as low as 3 mils with a
Premium Expanded, this is still marked as an Expanded in PCB Configuration.
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 Expanded
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 Expanded
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”.
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.
Go to Tools>Schematicß>PCB use Consistency Check to verify the design
when compared to your schematic. This
will output a report to review any inconsistencies between your Schematic and
PCB files. Both files will need to be
named the same other than extensions, and be placed in the same folder to have
PCB Artist recognize the files being connected.
Reviewing design rule check errors
Here are some effective ways:
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.
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.
Deleting my design rule checks
Go to Tools>Design Rule Check. In the Design Rule Check window, click the
Delete Errors button.
·
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.
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:
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 Expanded
Design Requirement.
c.
On the Board Parameters page, click on the V-Score
checkbox on the right.
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 Expanded 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).
It is possible but not recommended.
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.
Directions
for ordering a Student Special board may be found here: http://www.4pcb.com/media/Student%20Order%20Process%20updated%2004-14.pdf
Student
orders follow the same specs as 33 and 66 specials. You may order less than 4 boards on a student
order.
PCB
Artist does not interact with the Advanced Circuits Freedfm Service. Go to the Order
Processing section for how to submit your board order. The Design
Rule Check Section covers how to view any possible errors with the design that
may reflect on the manufacturability of the board.
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.
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 your
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.
Missing Bottom
Silkscreen on a Order
By
default PCB Artist will not order a bottom silk layer. This must be activated by checkbox in
Settings>PCB Configuration>Layers Section. If the bottom silk option is not checked then
it will not output, nor be ordered.
Where one gets a quote
through PCB Artist will depend on the type of board that is being ordered. A basic spec board will have the pricing
without shipping or tax in Settings>PCB Configuration, on the lower left. Basic spec boards have a discount for them as
they are ordered online and are considered a “Hands Off” board. The full price will be available when
ordering the board, after uploading the files, and selecting shipping
options.
Expanded spec boards use the
custom spec pricing matrix found online.
To get a quote on an expanded spec board, one may go to Output>Submit
Order. Because it is an expanded spec
board, the option “Get Quote” will be available, but not the Place Order
option. Make sure that you have no web
browser open. If you have an online
account, list the e-mail and password, then click the “Get Quote” button. If you do not have an online account yet
with Advanced Circuits, then please go here to sign up for one before trying to
order or get a quote: https://www.my4pcb.com/Net35/newcustomerform.aspx
33/66 Specials and Barebones
Boards in PCB Artist:
These
specials are slightly different in spec when ordered through PCB Artist.
To order
these specials through PCB Artist, they must be 7 mils (.007”) track and gap,
as they are considered Basic spec boards.
All other requirements are similar to the specials listed on their
respective pages.
Because of the nature
of promotion codes the pricing for them
will appear on the web ordering page after you’ve uploaded the files.
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.
Permissions accessing a file during installation
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:
A.
Run Regedt32 as was done in step a, above.
B.
Click on File>Import
C.
Locate the file from Step c above.
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.
Proxy firewall installation problem
Please send an email describing the issue to layouthelp@4pcb.com.
There is a link to that directory in Start
Menu>All Programs>Advanced Circuits>PCB Artist Data.
At this time only Windows systems from Windows 98
to Windows 7 are supported.
Downloading PCB
Artist through www.Download.com
Download.com
(Cnet) has included a mini downloader that will need to be installed before the
actual download of PCB Artist. More
information on the installer may be found here:
http://download.cnet.com/8301-2007_4-10010614-12.html?tag=ftr#CNETInstaller. This installer is an extra step in security
for Cnet. The downloader will also have
options for other software applications to be installed, that are not required
for PCB Artist to be downloaded and installed.
This extra software is not supported by PCB Artist, or Advanced
Circuits, so the user will download them at their own discretion. Some security software may flag the Cnet
downloader, and not allow downloading.
One will have to review their security if this is an issue. Contact PCB Artist support at Layouthelp@4pcb.com if you are still
unable to download from this location.
Optimizing the design for Advanced Circuits Assembly
Services
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.
Getting a quote for board assembly
Contact
your region’s sales representative for information regarding board assembly.
Creating a Bill of
Materials (BOM) and/or Component Positions Report
Assembly reports may be found under Tools>Reports. They are available in text or Excel
formats. It is up to the board designer
to review and correct these reports for parts information and placement.
If you
have a new question, please don’t hesitate to send it to Layouthelp@4pcb.com
