The Data Required section of https://www.protoexpress.com/products/no-touch/ is one of several places where Sierra asks for
“Gerber files in RS-274X format only (Extended Gerber) or ODB++ format. Do NOT use Gerber X2 format!”
My understanding is that Gerber X2 (and X3) are entirely backwards compatible.
Is this caution just to keep people from assuming you got the information from the attributes? Or is there some actual problem with the newer versions? If so, what?
That was originally added to our website when our CAM software did not support X2.
Currently, our CAM software does support X2. However, like any format, successful implementation requires two things:
Refining this process to ensure seamless compatibility can take time.
While our CAM software does support X2, we’ve found that it ignores all X2 attributes, meaning there is no actual benefit to sending X2 files. We don’t specifically check if files are in X2 format, but if we encounter issues when loading Gerbers, we may ask the customer to provide X1 files instead.
Regarding X3, we’re not sure of the current support status. we have submitted a query to our vendor and will provide an update once we get a response.
X3 is basically X2 plus component information, so if they aren’t using the attributes to grab layer information, I doubt they would do any additional work for components. For fabrication-only (ignoring assembly), that probably makes sense.
Grabbing the attributes (and/or gerber-job file) for your own online quote processing might simplify some submissions, but I obviously can’t tell how much friction that actually causes.
We would honestly prefer if designers would stop using Gerber and send us IPC-2581 files. Have you heard of this standard?
According to our CAM software technical support X3 is also supported. But as mentioned before all the attributes are removed so there is no benefit for us using X2 or X3.
I don’t think we have ever seen X3 data. If the customer wants to send us X3 it would be good if we could get a set of data just to see if we can really load it.
I have heard of 2581, though I hadn’t looked at it in nearly a year, and it looks like some of my memories were actually about ODB++, which some sources say it is based on. Maybe this year I’ll push through the admin barriers to get hold of the actual specification, or at least the schema, but I’ve already found and read the Gerber specification, because it was available.
https://www.protoexpress.com/kb/how-to-export-and-get-started-with-ipc-2581/ seems correct, but many of the advantages are more important to BigCorp than to a small team.
If it resembles any of ODB++, a typical large XML standard, or even the IPC-2581 partial sample files I’ve seen, then there is an awful lot of complexity, and incremental adoption may involve some bad compromises. That kind of complexity may even be the least bad option – it probably wouldn’t gain traction from Enterprise customers without kitchen-sink level support.
But for a small shop, incremental changes may be easier. Gerber isn’t really human readable, but it is viewable, and if you want to integrate a little more information at a time, the changes towards including more information are easy to verify.
@steve.carney To test X3, I think you’re looking for Official Gerber Format Website and its downloads page Ucamco | Downloads
Currently, I have to hit enter an extra time, and it refreshes with a list of downloadable files, including about a dozen test files.
They’ve been pretty careful to ensure that sending a new-version file to an old process won’t break anything. From section 6.9.1 of the standard:
“Component information was added in revision 2020.09, also called X3, by defining two new Gerber layers. By placing the component data in separate files, full compatibility is maintained: if one does not need component information, one can simply ignore the component layers. The new standard is therefore compatible with existing workflows. Legacy software can handle the CAD data with the new assembly information without change. Great care is taken to minimize the development effort by keeping the existing fabrication outputs in place and sticking to an existing syntax.”
For example, the file attributes (from X2) answer some of the questions customers otherwise have to fill out manually, and provide some integrity checks to prevent version skew. But if you just ignore them, you’re no worse off than before, except that a customer might wonder why they’re re-entering the data.
%TF.FileFunction,Copper,L4,Bot*%
%TF.FilePolarity,Positive*%
The top few test cases should test anything that changed with X3. Normally, the only difference will be two extra gerber files to represent the component layers. For example,
Gerber Layer Format - X3 - Kit Dev Coldfire Xilinx (zip)
includes kit-dev-coldfire-xilinx_5213-pnp_bottom.gbr which contains the X3 attribute value of “Component”.
%TF.FileFunction,Component,L4,Bot*%
Thanks for sharing this Jim. Ucamco downloads page is definitely a good place to access official Gerber test files. Appreciate the detailed breakdown of X3 compatibility.
For designers looking to test X3 integration in their process we still recommend running these test cases through CAM software and verify how the add. component layers are handled.
I do not see support for IPC-2581 in Sierra’s Instant Online Quote or Instant No-Touch Quote tools. It seems to me that, aside from quantity and lead time, all of the other fields in your quote form could be auto-filled from IPC-2581 data.
Yes, it’s only for custom quotes right now.