Altium Exports having problems with Drilling Files

[Aydin Yasar]

Hi All, 

I am quite new in here and also PCB designing. I am currently using Altium Desinger. 

As per my request from Simon, he shared me a guide which shows how to convert Altium Gerbers to Cirqwizard formats. (I have attached the file in here for everybody's reference.)

Here is my problem: 

When I export gerbers for engraving of top and bottom layer, I simply get the result properly. However when i follow the steps for the Drilling and Contour Milling, I don't get the required file format. 

Does anybody face similar issue or can anyone guide me through this? 

Thanks,

[Simon Salykov]

Hi Aydin,

Can you post an example of the drilling and contour milling files you are getting (together with either a top or a bottom layer)?

Simon

--
You received this message because you are subscribed to the Google Groups "cirqwizard" group.
To unsubscribe from this group and stop receiving emails from it, send an email to cirqwizard+...@googlegroups.com.
For more options, visit https://groups.google.com/d/optout.
<Altium_to_cirqWizard-2.pdf>

[Aydin Yasar]

Hi Simon, 

Here is the attachment. All my outputs (excessive ones as well) are in here. 

[Simon Salykov]

Hi Aydin,

Your drilling file is in Gerber format, whereas it's expected to be in the Excellon. That's why you don't get any holes. As to the contour milling, the layer indeed contains only the cross, as it is rendered in cirQWizard. I'm not familiar with Altium, so I'm not sure why you are getting these instead of  expected files. Hopefully someone using Altium can chime in with some idea.

Simon

<CirQWizard Conversion parameters.zip>

[Aydin Yasar]

By the way Simon, the same PCB has another problem with engraving. 

I attach an image for comparison. There are some insulation parts missed by the machine. I especially got the image on the right from cirQWizard to indicate the file is read correctly by the software. 

What would be the reason causing this? How can I fix it?

Thanks,

[Simon Salykov]

Aydin,

Tool path generation algorithm uses supplied tool diameter to calculate the offset from the traces. If the clearance between traces doesn't allow them to be separated with the tool of specified diameter without damaging the traces, cirQWizard won't generate the tool path there. After the tool paths are generated, you are supposed to review them before milling to ensure that you are actually milling what you were expecting. You can play with tool diameter parameter to balance clearance vs safety margin on the offset from the trace. You gotta stay within reasonable range, though - otherwise you'll mill the traces away. For 0.2-0.5mm tool anything less than 0.22 is asking for trouble.

Simon

On Mar 25, 2015, at 11:42, Aydin Yasar <aydin.y...@gmail.com> wrote:

By the way Simon, the same PCB has another problem with engraving. 

I attach an image for comparison. There are some insulation parts missed by the machine. I especially got the image on the right from cirQWizard to indicate the file is read correctly by the software. 

What would be the reason causing this? How can I fix it?

Thanks,

<PCB engraving errors.png>

[pra...@gmail.com]

hi

I do use Altium to generate the gerbers and nc drill files.
It took me a good day of experimenting to get it working as expected. Since then I made several boards without an issue.
The guide you posted is overcomplicated in my opinion.
Exporting the already generated gerbers and nc files from CAMstatic just for renaming the extension is over the top :)

However in step 2. and 10. be sure to always select milimeters and the highest resolution!
Also on the last tab (Advanced) for gerber export check the "keep leading and trailing zeros".
Same for the NC drill files export (step 10.) select milimeters, highest resolution and the the "keep leading and trailing zeros" option.

For some crazy reason (or bug in altium/cirqwizard) if I don't do the above steps I cant seem to get the drill file align with the gerbers.

But now everything is working.

Steps 3,4,5,6,7,8 is completely unnecessary. Since you are just generating the gerber files again from another program (CAMstatic) And it cannot do any good just introduce some error. If you look closely all the dialogue setting you are presented here you have had set in the altium export. Camstatic is a general gerber manipulation program. You don't need to use it for your purpose. Just rename the file extensions manually in your project output directory (or write a one click script)

Step 12 is confusing. Altium is too smart and can generate milling/routing files from board shape. But the output is excellon for a router (as it should be). For outline milling the cirqoid expect not excellon but gerber (surprisingly enough). So the way to go is to dedicate one of the mechanical layers for board outline. Draw the board outline there with a line width set the same as your milling tool (2.0mm) generate the gerber output with the rest and set the file extension what the cirqwizard expect it to be (*.ncl I guess)

[pra...@gmail.com]

I forgot to mention to uncheck "generate board edge rout path" in step 10.
This is not needed as I explained above, since the generated format cannot be used in cirqwizard and ou have to draw the board outline manually. At least it's much faster than using this generated path and convert it with black magic wizardry in CAMstatic (which I'm sure is possible). And as a bonus you can draw the separating tabs exactly where you want them.

[Aydin Yasar]

Hi, 

I am very very glad to receive your comprehensive answer. 

Actually last week we had a screen sharing session with Simon and resolved the problem together. He helped a lot... ;)

As you have just explained, most of the steps and even the selected layers in that document was redundant. So we have gone through generation of gerbers directly and simply changed the file extensions. Then for NC Drill file format we also changed Excellon units in CirQWizard as it was generated in Altium (I didn't know this particular detail was such important.) So we safely got our drill files. So far the selected resolution didn't cause me any trouble but for sure I will try your recommended resolution to check if it makes anything better for me. 

Finally for Contour Milling, again similar to your explanations, we went on 1 of the Mechanical layers and manually draw the lines to cut with 2mm thickness. When the gerbers are created this layer is automatically created as well. 

Cheers,

--
You received this message because you are subscribed to a topic in the Google Groups "cirqwizard" group.
To unsubscribe from this topic, visit https://groups.google.com/d/topic/cirqwizard/9nTzSagfYu8/unsubscribe.
To unsubscribe from this group and all its topics, send an email to cirqwizard+...@googlegroups.com.

[Aydin Yasar]

Hi Again, 

I would like to ask another help for the Altium Exports. 

Sincel last week, I have been trying to get proper Altium Gerber Export for my new PCB. However, no matter what i have done, my exported files cannot be shown on CirqWizard. I get an empty workspace on CW. 

The week before, I could at least get the right workspace and my imports were working except NC Drill files were never matching on the board even though I paid extra attention on the excellon units. 

Now, i cannot see anything on the workspace. 

Any information or guidance would be highly appreciated. 

Thanks,