I used to work also in the CAM area of various PCB manufacturers.

 

The ODB++ thing surprises me also....they were talking of this years ago.

 

The thing is....from my experience...extended gerber was sufficient for the CAM guy. It was a big improvement from the older non-extended gerber.

Obviously the biggest problem with the older gerber was the aperture lists. Quite a lot of the times these had to be manually typed in and because of this, most times, 2 guys were needed.

One to read, one to type, then double check....lots of room for error.

 

There could be that there are still minor problems reading in the the drilling data.

Again from my experience in the past, this data could come in all sorts of formats (Excellon...Sieb&Meyer....then...2,4...2,3...3,2....inch.....metric...leading zero or trailing zero suppression etc....).

This required some kind of trial and error. And if all else failed....create this file from the pads off one of the layers.

 

Regarding modifications...again from my experiences...

Via hole diameters were always preferred that they could be left up to the manufacturers discretion so as to optimize the annular ring and therefore registration.....

Often the finished diameter, detailed on the drill drawing, would be considered as the DRILL diameter.....therefore 0.10 to 0.15mm smaller for the FINISHED size.

 

Small changes.....we are talking of pad small pad increases etc.....could be changed without notification....depended much with the client....some were more picky than others....

 

Usually any type of track movement or major errors were reported back to the designer so that he/she could modify the source files.

 

Most times the apertures for the solder resist layers were "Blown" without notification.

If asked it was always stipulated that the solder resist apertures be one to one with their respective pads so then after the aperture increases they would be uniform in size throughout the board.

 

Regarding silkscreen...

If the board was going into quite high volumes then there was the need to shift the identifications of the components slightly so that they wouldn't get clipped....and therefore be illegible.

 

Small volume prototypes...most times....no modifications....and it was just clipped.

 

Etch compensation was always applied.

 

If there was a modification that notification was needed....usually then....all modifications were reported....even the slight ones....but generally....not too much detail.

 

Anything critical....the production was put on hold until further notice from the designer.

 

It has been quite a few years since I was in this field.....some things and approaches have most probably changed.....and also these approaches could change from manufacturer to manufacturer.

 

Now I'm a PCB designer this experience has helped me greatly in some aspects of my designs. And so far, fingers crossed, no questions have been asked.

 

The opportunity presented to you Jack, I would recommend very much.

 

Just one day sat with an experienced CAM guy is very helpful.

 

Paul Di Marcello
PCB Design Engineer

Pepperl+Fuchs Elcon srl
Via delle Arti e Mestieri, 4
20050 Sulbiate (MI) ITALIA

---

From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Jack Olson
Sent: mercoledì 14 maggio 2008 22.29
To: [log in to unmask]
Subject: [DC] FAB:CAD2CAM

 

I've recently had the opportunity to spend some time with "the CAM guy" at our primary circuit board supplier, and now a magazine has expressed an interest in publishing an article about what happens to data as it moves from CAD through CAM. If any of you are involved in this process, here is a golden opportunity to voice your concerns (or your "wish list"). I already have my notes for what happens to OUR data, but I would like to be more generic for the magazine.

 

If you aren't doing CAM work but know someone who might like a shot at this, PLEASE forward this to them.

 

The most surprising thing I learned this week was the extremely low percentage of jobs being submitted in an intelligant format. For example, we've been told for years to move to something like ODB++ or GENCAM, but I'm hearing that maybe only a few percent of the jobs are anything other than regular old Gerber. Is that true? Would it help you significantly to get some alternative to Gerber?

 

I'm also interested to hear anyone's thoughts on the note that can be found on many drawings that says:

"DATA SHALL NOT BE MODIFIED WITHOUT WRITTEN APPROVAL".

Where do we draw the line on that?

Plot film with data "AS IS"?

How does it apply to

etch compensation?

removal of non-functional pads? 

teardropping? 

silkscreen clipping?

What is "standard" editing, and what really should be pre-approved?

 

We've been told to always place the origin on a tooling hole. Does it really matter?

Would you rather have the soldermask 1:1 with the pad size and enlarge it yourself?

Would it help you much to have positive planes drawn with unique aperture sizes?

Does the format matter? inches? metric? consistent with drill?

Would it help to have better README files that explain more of our intentions?

(like a known netlist discrepancy, for example)

 

What do you wish more people would do to make your life easier?

 

Maybe its inconvenient to answer so many questions, but if we have a chance to teach designers what we want, shouldn't we try?

(I'm gonna write it with you or without you, so don't complain if what gets published is off-grid)

Also, If I didn't ask the question you want to answer, don't hesitate to add to the list!

 

If YOU were King of the World for a day, what would you change?

 

Thanks in advance,

I'll try my best to write a fair and thorough article

 

Jack

[log in to unmask]