CAM-350 questions

[randychase]

Hi.

I am auto-importing into CAM-350 from PowerPCB. That works fine for the gerbers, but I get some errors with the NC drill files.

First I get an error message that none of the drill tools are assigned. Why?

Secondly, the drills are not aligned with the gerbers. They are in odd clusters that don't seem to make sense.

My NC output is as follows:
Absolute coordinates
ASCII
English
3 5 digits
Trailing zero suppress
Excellon format

Pretty much the default from PowerPCB and I have never received a complaint from a manufacturer, so I left it alone.

Thoughts?

[randychase]

CAM-350 is expecting the NC drill as 2:4 instead of 3:5.

I can change the output of PowerPCB CAM or I can delete the NC drill stuff and then import the drill file again with the proper settings.

It's still not aligned, even though I gave it the same offsets. But aligning it is pretty simple.

[Mark Larson]

Import all Gerbers except the NC, then once you have the Gerbers in, place the origin at your PPCB origin, then import your NC

For the NC Tool Table you can use the script PADS Drill.scr, it works pretty slick. Why they don't have this as part of the AutoImport process ...who knows

[randychase]

Mark, can you explain a little more about the script? Thanks!

[Mark Larson]

The script is straightforward:
Macro-Play-Pads_drill (should be in your Scripts directory of CAM350, if not browse to it)-when run a dialogue box will appear, browse to the drl.rep file that was created in PowerPCB CAM.

To check to see if the macro did the trick, Tables-NC Tool Tables if the size and column match your report file, you are OK

Instead of using the script, you can manually edit the info at this table.

[randychase]

Thanks Mark. If I do this enough, that will really help.

Anyone know if I should look into version 7.5?

[Mark Larson]

Originally posted by randychase
CAM-350 is expecting the NC drill as 2:4 instead of 3:5.

I can change the output of PowerPCB CAM or I can delete the NC drill stuff and then import the drill file again with the proper settings.

It's still not aligned, even though I gave it the same offsets. But aligning it is pretty simple.

In case you haven't caught info on the list server you might like to know there is an easier way. I had tried to get CAM 350 to read the drill sizes before but it was coming in 1000x and some sizes were really wacked. Since people on the listserver were apparently successfully reading the drill sizes correctly I took another look, here is what you can do and also how I cured my scaling problem:

Go into CAM document for your NC Drill - Edit - Device Setup - Format String - Type - Tool Section Start - add C@d to string, you do not need F@fS@s (feed & speed) but its OK to have it there, the minimum string, the info that is important is: T@tC@d

why it didn't work before for me was I was outputting 3,5 and changing CAM350 from 2,4 to 3,5

to fix make sure the format of both Excellon & Drill Listing under Format is set to 2,4, also make sure the other settings for Coordinates & Units match CAM350 settings, I was doing opposite, trying to match CAM350 to PowerPCB

AutoImport into CAM350 should now read in drill sizes corretly, and if you use offset for generating CAM info, they will be alligned as well, no more manual manipulation of data! Also doing this way allows easy panelizing, import Drill data again, import Gerbers again (yes to merge), repeat as necessary, I find it easiest to relocate origin in CAM350 before each drill data import to bring in data to correct spot (don't need to do that on original AutoImport), then when I bring in Gerber can use 0,0 as selection point. Relocate origin when done

now a question: does anybody use CAM350 to output a "drill tape" rather than using the output from PPCB? any problems from vendors? we always give the data from PPCB

[Jason Roetz]

I've always exported NC drill info from CAM350 rather than Pads. Never had a vendor complain yet.

Jason

[ltrakal]

So Mark, it seems to be that you followed my steps to panelize the boards. I was wondering if you could do it or not.
Yes, I generate the drill file and the final gerbers from CAM350 and no problems at all.
By the way I always work in metric so having this as experience with several board shops I import and export with 3:5 Leading settings, now they like 2:4 Trailing for Enlish designs. Why is that? I don't know.
And I never use autoimport, it doesn't work very well I alwasy use import gerber data and thend the drill file, with offset settings in powerpcb they all fall at the same spot.

Laszlo

[Mark Larson]

[QUOTE]Originally posted by ltrakal
[B]So Mark, it seems to be that you followed my steps to panelize the boards

thanks for the help, yes it worked , I should point out that I am made a panel of 2 different boards, so first I would AutoImport the first, then do the Import Gerber as you suggested. But now I am wondering if there is any problem with just doing a copy of the 2 boards to get 4, 6,... or if you are panelizing one board, doing a single Import, then do a copy for the rest. The copy method seems the easiest, but don't know the downside.

I have used the macro with V6 CAM350 in the past to panelize, now this way, I am wondering what the panel editor does that the other 2 methods do not? Anybody know?

[Jason Roetz]

We do very little panelizing, but when we do, I just import the one and then copy and paste the rest.

Jason

[ltrakal]

Originally posted by Mark Larson
[QUOTE]Originally posted by ltrakal
[B]So Mark, it seems to be that you followed my steps to panelize the boards

thanks for the help, yes it worked , I should point out that I am made a panel of 2 different boards, so first I would AutoImport the first, then do the Import Gerber as you suggested. But now I am wondering if there is any problem with just doing a copy of the 2 boards to get 4, 6,... or if you are panelizing one board, doing a single Import, then do a copy for the rest. The copy method seems the easiest, but don't know the downside.

I have used the macro with V6 CAM350 in the past to panelize, now this way, I am wondering what the panel editor does that the other 2 methods do not? Anybody know?

Oh yeah, you are correct, if you need more of the same boards that you imported already you only copy those, select the window command and that's it.
One thing though, remeber to have all the layers on of the board you are selecting.
So you use verison 6? That macro won't work on verison 7?
The panel editor on version 7 I think is more complicated to use. And the downside of useing the merge command is that I heard from one guy that does this for living, he panelizes boards everyday, that he started to using it on verison 6 but somehow the program screwed his layers so after hearing that from somebody that uses the software everyday I won't use it plus the import gerber command works cooll and it lets you place the board wherever you want.

Laszlo

[Mark Larson]

The macro does not work on version 7, here is the error:

"This macro is trying to execute a command (panel_spread@) which is not supported by CAM350."

Line 340:
panel_spread@ 0,0

As for the Import-merge method, I can see how if you are not careful it would be easy to goof up layers.

[Tom]

I believe that DownStream Technologies is has removed the Panelization feature for the latest revision of CAM350 because they refer to that feature as a "Manufacturing Feature".

I had a conversation with them and mentioned that we never use the Panelization feature, so could we get a discount and not pay yearly maintenance for this feature and they replied that that was common with many PCB designers using CAM350. Hardly any PCB Designer uses this feature so why pay for it (over & over again).

If you want it, pay the extra to get it and don't penalize the people who don't want it.

[Boarddesigner]

Originally posted by randychase
CAM-350 is expecting the NC drill as 2:4 instead of 3:5.

I can change the output of PowerPCB CAM or I can delete the NC drill stuff and then import the drill file again with the proper settings.

It's still not aligned, even though I gave it the same offsets. But aligning it is pretty simple.

I have tried to do the process of importing drills as suggested but am getting this error:

ERROR (21): On line 146 of c:\program files\downstreamtech\cam350\scripts\pads_drill.scr
Description: "Input past end of file"

Line 146:
input #1, Tool%(C)

Where am I going wrong?

Boarddesigner

[H.Tikkanen]

Excellon format is very old. If specified to "metric", 3.3 is assumed. It is also possible to set parameters in PowerPCB so that it includes drill sizes in the actual drill file. Thus it is possible to use CAM350 AutoImport and get the drill sizes and units correctly every time without manual intervention or macros.

Description of this can be found from:
http://www.designsystems.fi/tuki/powerpcb_postprocessing_parameters.pdf and
http://www.designsystems.fi/tuki/tulostusparametrit.htm

The pages are in Finnish (sorry), but there are screenshots in the pdf file which should clarify. If there is interest I could provide this also in English(?).

Hope this helps.