Need help? Get in touch.
Cropping PCB Elements
To ensure that elements from different PCBs do not interfere with each other during our batching, panelizing, and manufacturing process, we may automatically crop elements from a PCB which lie outside of the board outline.
For some layers, this isn’t a serious problem. Silkscreen or solder-mask features which are outside of the border are automatically and silently removed, and do not normally have an impact on the final result. For other layers such as copper and drills, this may result in your board not being manufactured as you expect. In these cases, we provide you with an error message indicating that we have cropped features from your board which were outside of the board outline.
Check in an external viewer. If you are having cropping issues, we suggest that you look at the gerber and drill files that you have uploaded with a gerber viewing tool. There are several available at little to no cost. We recommend the open source tool Gerbv for this purpose. The home page for Gerbv is http://gerbv.geda-project.org, and the windows version can be found at https://sourceforge.net/projects/gerbv/.
In any case where you see a message that elements are cropped, the board should be examined very carefully before ordering. If you have any questions about why your specific board has elements that have been cropped, please contact us
Common Drill Errors
In the case of drills, this is almost always an issue that needs to be addressed before you order the board. Issues which can cause cropping of drills include:
Incorrect Origin for Drill files
The drill file must use the same point for the origin as the Gerber files for the other layers. Failure to do so will result in drills not lining up with other features in your board, and drills getting cropped. The following images are from Gerbv:
Here we have a case where the Gerbers are using the lower left-hand corner of the board as the origin, while the drill file is using the center of the board as the origin. The will result in a number of the drills being cropped, as well as the remaining drills being in the wrong location. The fix for this is again to check your export settings for the drill file when exporting the drill file from your EDA tool.
Incorrect Number of Digits in Drill File
The specifications for the Excellon file format state that in Inch mode, there are to be 2 digits of precision for the integer portion of a coordinate, and 4 digits of precision for the decimal portion. Producing a drill file with more or less digits of precision will cause errors when it is parsed, resulting in many drills getting cropped. This is rarely an issue in metric mode where the coordinates typically have the decimal point included.
Here we have used the Zoom to Fit feature of Gerbv to show all of the features that have been loaded. Because the drill file has too many digits of precision, the coordinates of the drills are all off by a factor of 10, placing all the drills outside of the board outline. They will all be cropped when uploaded to MacroFab. To correct this, insure that you are using the correct number of decimal places when exporting the drills from your EDA tool.
Drills Included in EDA Symbol
In some cases, the EDA tool may define a symbol which includes a drill. An example of this is a TO220 which includes a drill for fastening the part to the board. If this symbol extends past the edges of your board placing the drill outside of the borders for your board, this drill will be cropped, and you will receive a message to that effect. In this case, if your plan is to mount this component vertically, and do not need the drill in the board, then you may order this board with the cropped drill without any issues.
Common Copper Errors
In the case of copper layers, this is often an issue that needs addressing. There are exceptions, however where the cropping will still produce a board that will be what you expect. Common issues that cause cropping of copper layers are:
Some EDA tools include a title block on every layer (including copper layers) which lie outside the board outline. Ideally, when exporting the gerbers from your EDA tool, you should indicate that the title block should not be included. However, if they are included on your copper layers, they will be cropped, resulting in the error message. If the only elements that have been cropped are title blocks or other documentation outside of the outline, then the board may be ordered without issues.
EDA Symbol Extending Beyond Board
Like we saw in drill files, in some cases, the EDA tool may define a symbol which includes copper as part of a symbol. In some cases, this copper is for a ring around a drill as is the case for some TO220 symbols, or might be for a heat-sink, or other purpose. If this symbol extends past the edges of your board, and places copper features outside of the borders for your board, these features will be cropped, and you will receive a message to that effect. In this case, if your plan is to mount this component vertically, and do not need copper features which have been cropped, then you may order this board with these features cropped without any issues.
Let’s look at a common issue with symbols extending beyond the board outline, as shown in Gerbv.
The transistor shown here is extending past the board outline, and you can see that there is a drill along with a copper ring around drill. If only the silkscreen were extending passed the outline, it would be silently cropped. However, because of the drill and copper beyond the outline, this design will produce the cropping message when uploaded to MacroFab.
As you can see, the silkscreen has been trimmed to the outline, and the drill and copper elements that were outside of the outline have been removed. In this case, the intention of the designer is that the TSO220 package will be mounted vertically, so the fact that the drill and copper has been cropped will not impact the project.