Here’s a PCB ordering tip from Advanced Circuits:
CAM hold can cause your order to be delayed, but you can avoid CAM hold by using our FreeDFM™ tool.
Save time and money on your PCB orders with this design for manufacturability tool, which you can use as many times as you want, free of charge. The most effective way to avoid having your order go on CAM hold is to take advantage of FreeDFM™.
FreeDFM.com will give you the following benefits:
- Free printed circuit board design file check for manufacturability
- FreeDFM™ checks to make sure we have the files and data necessary to build your PCB job
- The Results are e-mailed to you in WITHIN MINUTES.
- FreeDFM™ gives you a graphical report, showing any potential issues with your Gerber Files' detail as to their nature and location.
- Reduces possibility of CAM Hold issues with your PCB order after it is placed.
- Enables 48% faster total thru-put from order placement to shipment
- Also provides a price quote with your choice of printed circuit board turntimes.
- Advanced Circuits will even pay you up to $100 to use FreeDFM.com when you place your order.
FreeDFM eliminates those problems that can translate into days lost on the schedule
When I provide Gerber files that have been “pre-checked” by your FreeDFM service, I know my clients will not have unwelcome delays getting their boards produced. FreeDFM eliminates those problems that can translate into days lost on the schedule." - R.P., Capital Products Design
Go to www.FreeDFM.com Now to upload your files and avoid delays on your printed circuit board orders.
Creating Gerber files that accurately reflect what you want manufactured is a challenge no matter how long you have been a PCB designer. However, by learning from colleagues or other sources and avoiding the most common mistakes, you can speed up the turnaround time, reduce the chance of printed circuit board orders placed on hold, and complete your projects faster. The following list reviews the "Top Fifteen Most Common Mistakes" made with Gerber files and how you can avoid them.
1. Missing Aperture List
Your Gerber files specify what to do and where. Your aperture list specifies what size and shape of an object to draw at a give location (Dcode). A single comprehensive aperture list for all layers should be sent with your Gerber files, rather than a separate aperture list for each layer. Please note: An aperture list does not need to be sent with 274X format files. If you send 274D format, we use your aperture list in combination with your Gerber files to create your artwork.
Requirements: One comprehensive aperture list for all layers, English Units. Please do not modify the aperture list your software outputs. An aperture list does not need to be sent with 274X format files.
Resolution: All layout packages which output 274D also output an aperture list. Common extensions include .rep, .apt, and .apr. If you have difficulty outputting an aperture list, please send 274X format.
2. Missing Drill File
Drill files are used to determine what size holes to drill and where. Plated and non-plated holes can be included in one drill file, with plated and non-plated holes having different tool numbers.
Requirements: Excellon Format, ASCII Odd/ None, 2.4 Trailing Zero Suppression, English Units, No Step and Repeats.
-Gerber drill files may be accepted if plated versus non-plated holes can easily be determined.
Resolution: Nearly all layout packages will output an Excellon drill file. If you cannot generate one, we can in most cases create one from your fabrication drawing for an engineering fee.
3. Missing Tool List
A tool list is used in combination with your Excellon drill file to create your drill. Your drill file specifies where to place the holes. Your tool list specifies what tool to use. A tool list should be embedded in your Excellon drill file or sent as a separate text file. Using a tool list provided on a fabrication drawing is not preferable, as it eliminates many of the automatic verifications and makes data entry errors far more likely.
Requirements: Tool list embedded in Excellon drill file or sent as a separate text file.
Resolution: If your layout software will output an Excellon drill file, it will also output a tool list. Common extensions include .tol and .rep.
4. Missing Gerber Files
Many times people submit orders and forget to attach their Gerber files.
Requirements: Gerber 274X or 274D, English units are preferable.
Resolution: ODB++ files are acceptable; however, these files should be sent to [email protected]. It is possible to convert many other file formats to Gerber. Please send your non-Gerber formats to [email protected].
5. Insufficient Annular Ring
An annular ring is the donut ("annulus") created when your drill pierces a copper layer. It is defined as the radius of this donut. For example, a .030" pad with a .020" hole would have a .005" annular ring. This is required to allow for complete plating on vias, as well as solderability on component holes. Many times people do not allow for the proper annular ring requirements.
Requirements: A minimum of .005" annular ring for vias or a minimum of .007" for component holes is required for manufacturing. Advanced Circuits requires that vias with connecting traces have a pad that is 10 mils larger than their drill, and component through holes with electrical connections have a pad that is 14 mils larger than their drill. Tooling holes with no electrical connections may have 0 mil annular ring.
Resolution: All layout packages provide this as a DFM check. Setting a sufficient annular ring in your layout software is the preferred method in order to maintain proper copper spacing.
6. Insufficient Copper Trace Width/Spacing (Trace and space)
Copper spacing is the minimum air gap between any two adjacent copper features. Trace width is the minimum width of a copper feature, usually traces.
Requirements: A premium is charged for trace width/spacing less than .007".
(We can process .004" for 1 oz. CU. finished (outer layers) and .5 oz. CU finished (inner layers).
For 1 oz. finished copper weight (inner layers), the minimum trace width/space is 0.005"
For 2 oz. finished copper weight (inner & outer), the minimum trace width/space is 0.006"
For 3 oz. finished copper weight (inner & outer), the minimum trace width/space is 0.010"
For 4 oz. finished copper weight (inner & outer), the minimum trace width/space is 0.012"
Note: Advanced Circuits does not offer weights such as 1.5 or 2.5 ounce finished on standard and custom spec orders.
Resolution: All layout packages provide this as a DFM check. Setting sufficient trace width/ spacing in your layout software is the preferred method. Trace width and spacing push and pull against one another, so changing a problem area may require rerouting traces, adding vias, or moving components.
7. Insufficient Inner Clearances
Inner clearance is the minimum distance from the edge of a hole to any adjacent, unconnected, inner layer copper. Sufficient inner clearances help ensure that your drill does not cause shorts to your inner copper layers. This is important for both plated and non-plated holes, as non-plated holes may either cut into an adjacent trace or cause shorts during assembly.
Requirements: A minimum of .010" inner clearance is required and .015" is preferred.
Resolution: Most inner clearance issues can be resolved if negative image inners are provided, but it is preferred to not modify these. Setting these clearances in your layout software is the preferred method, as this will maintain intended connectivity. While most layout packages provide this as a DFM check, not all do. Those that do not can usually be manipulated to check for this violation by setting spacing and annular ring higher.
General guidelines: Spacing + Annular ring = Inner clearance. Another trick that can help resolve problem areas is to move the affected traces to outer copper layers, where this is not an issue.
8. Missing Board Rout Outline
A board outline/rout path needs to be included with your file set. Gerber files are preferred, but a dimensioned drawing will work provided it is simple to make an outline from, and we can determine how to align it correctly relative to the circuitry. As long as we can identify a line that is the perimeter of your board and it matches your ordered dimensions, we will use it for your board outline.
The most common method that customers use for communicating how to cut out their board is to place a 10 mil line on the top copper layer around the perimeter of their circuit, centered on where they want us to cut. We prefer a 10 mil wide line on the mask layer. The edge of the router bit will cut to the center of the given line unless we are told otherwise in the notes. Some customers put the board outline on all layers.
The board outline/route path can be found on an assortment of layers depending on the PCB software program used. We commonly see the board outline on one of the mechanical layers (.gm1 to .gm10). Some software packages have the outline on the .out (outline), .mil (milling layer), .fab (fabrication layer) or the drill symbols layer. The drill symbols layer usually has the drill chart, symbols showing where the drill hits are and the board outline along with any internal cutouts for the board.
Warning: GKO layers will NOT be used as an outline to cut out your board. The GKO layer is meant to be the keep out layer. If this is the only outline provided, your job will be placed on hold and we will ask if you do want us to use the GKO outline as your board outline.
Note: With many software packages, the "outline" is seen on all layers (as a global layer), but will commonly not appear in the outputted Gerber files. Gerber file viewers can be used to check if your software is placing the board outline in your files.
Resolution: We can make an outline for you, but we will need your permission to do so.
If your board is a perfect square or rectangle, we can make the outline if we know the exact dimensions and any corner relative to a feature such as the center of a tooling hole. Alternatively, if we know your board is a perfect rectangle and we know the x and y dimensions, we can center this rectangle around your design.
Rout (Board Outline) tolerances
The Outer Layer Tolerances on Standard Spec defined boards is +/- 0.010"
(+/- 0.005" available for Custom Spec upon request)
9. Exposed Copper may be Viewable on Board Edge or Inside Cutouts or Non-Plated Drills
Exposed copper may be viewable on the board edge due to copper being to close to the rout line (board outline) that we will use to cut out the board(s)
Single boards, Tab-routed arrayed boards and boards with cutouts:
Outer layer copper should be 10 mils away from the center of the board edge to prevent exposed copper. Copper within 10 mils of the center of the rout line may be exposed and viewable from the board edge.
Inner layer copper should be 15 mils away from the center of the board edge to prevent exposed copper.
Scored boards: (0.062" thick boards):
Outer layer copper should be 15 mils away from the center of the score line to prevent exposed copper. Copper within 15 mils of the center of the scoring line may be exposed and viewable from the board edge.
Inner layer copper should be 20 mils away from the center of the score line to prevent exposed copper.
For 0.093" thick boards, add 5 more mils of space than described above.
For 0.125" thick boards, add 10 more mils of space than described above.
Non-plated holes can have 5 mils spacing from the edge of the drill to the nearest copper.
Resolutions: Either 1) Pull back your copper from the danger zones (as mentioned above) to assure that there will be no exposed copper, or 2) Put a note in your order (such as a readme.txt in with your file set) that tells us that exposed copper is intended and/or expected. Or 3) Put a note in your order telling us that you would like us to pull back any copper that might be in these danger zones so that there will not be any exposed copper viewable when the boards are completed.
Note: If there is copper trace that will be clipped due to being too close to the board edge, Advanced Circuits may choose not to run the board because of the possibility of severing/lifting the trace.
10. Cutouts, Non Plated Slots, Plated Through Slots, Internal Routing, Milling Channels Specifying cutouts (internal routing):
Customers can specify cutouts in many ways. We commonly see cutout information on one of the mechanical layers (.gm1 to .gm10). Commonly placed on the .mil (milling layer), .fab (fabrication layer) or the drill symbols layer. The drill symbols layer usually has the drill chart, symbols showing where the drill hits are and the board outline along with any internal cutouts for the board. The best way to assure that your cutouts get included is to have the word "cutout" inside of the cutout, or an arrow pointing to the object to make it clear that it needs to be cut out.
Slots (minimum width allowed):
- Advanced Circuits minimum width for non-plated slots is 31 mils (0.787mm). Bit radius 16 mils (0.394mm)
- Advanced Circuits minimum width for plated slots is 26 mils (.660mm) Bit radius of 13 mils (0.330mm)
- Plated slots are only allowed on custom spec orders. Slots are not allowed on bare bones, $33 and $66 specials.
- Slot locations can be communicated to the engineers in many ways. A separate layer with 10 mil outlines of the slots is preferred, but it is possible for us to connect end drill hits that have a diameter of the width of the slot if we can determine which drills need to be connected to form a slot (such as a drill symbols layer with a drill chart).
- Plated slots should have copper over their locations on the copper layers, and should have at least 7 mils of copper overlap per side.
11. Drill hits that are small and too close to other small drill hits.
Advanced Circuits requires a minimum of 10 mil spacing (edge to edge) between drilled holes that have a diameter less than 65 mils. Otherwise drill bits can break during high speed drilling.
12. Full Fabrication Print required for Custom Spec Orders over $2k.
Advanced Circuits requires that Custom Spec orders over $2,000 have a fabrication drawing, (or a waiver that the fabrication drawing is not required). This fabrication drawing may be in either Gerber or .pdf format and should consist of drill chart with drill count, drill symbols, drill tolerances, board dimensions, and any fabrication specifications that are required. A drill chart has all the holes listed, their size, the quantity, whether they are plated or not, and the associated hole tolerance for each. At a minimum, the fab drawing should have a drill chart and a drill drawing.
Please note: If you request to waive this requirement, all drills that cannot be determined as to whether they are plated or unplated will be produced as plated.
Also note: A waiver for the fabrication print requirement can be selected during ordering:
Click Here to view a screen shot of the "Order Details"
"1-edge" goldfinger is one group of card edge fingers, component and solder side. "2-edge" golfingers is two sets of groups of card edge fingers, component and solder side of the board.
14. Mismatches between what has been Ordered and what is found by the CAM Engineer in the Fabrication Drawing, Gerber files, or Readme.txt files:
If there us a disagreement between the order information and what the supplied documentation calls for, this can cause a hold on the order.
Resolutions: Verify that your Fabrication drawing notes match what is on the order, if they do not, produce a readme.txt to state that what notes do not apply to the current order.
I.e. if the fab calls for red soldermask, but you have ordered and are ok with green soldermask color, then place a note in the readme.txt stating that the green soldermask color is an acceptable substitute for red.
Verify that your boards specifications match your order type:
15. Board or an Array Dimension Conflict:
If the ordered board dimensions do not match the size of the board seen in the Gerber files or other documentation, the job may go on hold until these discrepancies are resolved. Standard spec orders may receive an FYI and be run with the dimensions found in the Gerber files, if the values are close.
Resolution: Accurately measure the greatest X dimension and Y dimension (extends) of your board, or add a note in the readme.txt file that we should run with dimensions found in the Gerber files.
16. Layer order Stackup Information:
If your board is greater than 2 copper layers, we need to know what order the layers must be stacked up, so you should list the order the layers should be stacked up in the fabrication notes or your readme.txt file.
You can also see our CAM Procedures