Drill Symbols file corrupt

[EEGlenn]

I have recently completed my first project using Ultiboard 10.1.1. I have used other software in the past, but my current employer just received the Circuit Design Suite a few months ago. When exporting the Gerber files for manufacture, the drill symbols file seems to have gone crazy. My project has less than 100 holes to be drilled in two through drill operations. Some how the file seems to have overlayed one drill table on the other and came out with nearly 4000 holes. Many of which are actually OUTSIDE of the board boundary. Any ideas on how to correct this. I have modified the project and created two new sets of Gerber files with the same results. The NCdrill files and the file summary report look good, but the symbols file goes crazy every time.

[yyao]

Hi there,

This seems to be quite strange. I tried this in Ultiboard 10.1.1 and couldn't see this problem. Would you mind posting any small portion of your design which can trigger this behaviour? Would you mind posting both the Ultiboard project file (ewprj) and Gerber (and drill file if neccesary)?

Thanks.

[EEGlenn]

Unfortunately, that is not possible, due to customer confidentiality. I have not been able to identify the "trigger" as there is no trouble in the project. The Gerber files all look good except the Drill Symbols file. That I can attach if it will help. I have other projects in developement and need to know what is causing the glitch.

[yyao]

Hi there,

It looks like you are using blind or buried vias in your design. Not all vias in your design connect the same layers. Because of this, Ultiboard is exporting a seperate drawing for every layer to layer via combination that you are using in your design. There are 3 of these combinations in your design and Ultiboard is exporting 3 drawings. All 3 drawings are exported in one drill symbol file.

Most gerber viewers don't support the LN command (layer name) which is used to indicate multiple drawings in one gerber file. Hence, it appears to the user that there is overlapping or incorrect text. This is what your board house may be seeing. However, the built in gerber viewer in Ultiboard handles this command correctly. Simply, open the gerber file in Ultiboard. You may have to change the colour of the imported layers to be visible. You can set the visibility of each of these drawings by setting the check boxes in the Layers list.

In short, what you are seeing is correct behaviour. Just make sure that you are using a gerber viewer that supports multi-layer files.

Hope that helps.