ultiboard 12 - bug exporting gerber X

[Tonitos]

Hi,

I believe there is a bug in Ultiboard 12, gerber X handling.

If you export a layer in gerber X format, the files are generated and correctly interpreted by ultiboard 12.

The bug becomes apparent when one opens the created gerber files on third partie software or even on Ultiboard 11.

So far I have seen missing power planes and missing nets when on top of power planes.

In the PDF atached on the bottom layer you can see short circuits between the power plane and some nets

On the top layer PDF the nets are missing.

I share a gerber file, generated on Ultiboard 12 as an example an PDF files for it as seen by Ultiboard 12 and 11.

Any ideias what may be going on?

[Tonitos]

I now attach what Ultiboard 12 sees.

I have also found this post. This leads me to believe that the problem may be recorring.

[Tonitos]

The problem still exists on Ultiboard 13.

[stressed_user]

Hi,

I still work with the v10 version...

When I have issues with gerber output, I can usually solve it this way:

the last thing to do before exporting: force a Netlist / DRC check (under the tab design)

It always helps for me...

good luck!

[Tonitos]

Hi,

All test are OK, no errors.

The problem is in the generated gerber.

There is a problem with Ultiboard 12 and 13.

Best regards

[Tonitos]

Hasn't anyone faced this problem as well?

[Tien_P]

Hi Tonitos,

Did your board manufacture indicate any problems with the gerber files?  What third party tool are you using?

I imported your gerber top file into two gerber tools, Viewmate (free viewer available) and GerbTool and both looks much different than what the top layer looks like in Ultiboard 11.  We are not getting report about gerber problems from Ultiboard 12 and 13.

.

[stressed_user]

And I just opened it with the Altium viewer, no problem there...

[Tonitos]

Hi,

Yes, my colleague in charge of producing the PCB noticed something was wrong.

After viewing the files on his software e found that they appeared in a different way than the one I intended.

I then tried opening the files in different softwares.

I'm convinced there is a bug because Multisim 11 and Multisim 12 differ in the way the gerber is interpreted.

Multisim 11 agrees with the third parti software my colleague uses.

I can share the Ultiboard file in Multism 12 if you would like.

Regards,

[Tien_P]

Hi Tonitos,

There were changes to the gerber export when Ultiboard 12 was released. In Ultiboard 11 and older, copper areas were created using lines but in Ultiboard 12 and 13, copper areas are created using polygon shapes.  The commands used in V12 are standard gerber commands and your tool should support them.

In the old gerber export, your copper top will appear as 1 layer in your gerber tool, but the new format will create multiple layers. For example, the copper top layer you attached previously generates three layers a gerber tool. In attached screen shots, layer 1 shows most of your board covers, layer 2 removes clearances around the pads and traces, layer 3 adds the traces and pad back. I noticed the layer 1 is the same as your pdf attachment screen shot, check with your colleague if all layers are turned on the gerb tool.

If you like me to look at your design, send me a private message with your email address.  I will send you an email so that your design will remain private.