What process are you following? PADS doesn't have a Gerber viewer, unless they added it in 9.5.
I use Viewmate to verify my Gerber files; others like GCPrevue. I prefer to get a 'second opinion' about the Gerber files by reviewing them with something other than the tool that created them.
This link is what I found on SupportNet regarding viewing my photopots in PADS Layout 9.5.
Well that is a 3D viewer for the PCB and not a gerber viewer. Totally different thing. PADS does not have the capabilty to import, open, edit or view a gerber file.
If you need/want to view your gerber files you will need to either download a free viewer like Viewmate from pentalogix or GCPReview as mentioned,
or buy something like Wise Gerbtool, CAM350 etc. But Viewmate is free and works very well for viewing for verification. Which as mentioned would agree
I also like most prefer to use a different tool than what produced the gerbers for viewing.
PCAD, which is what I used to use, had a Gerber viewer built in, so I never had to use a separate viewer application.
I wonder why Mentor tells you to use this procedure?
There was no mention of this being a 3D viewer.
I'll check out Viewmate and GCPReview.
OK I see what is going on now.
When I used that link within my email it brought me to a 3D viewer instruction, however when I launched that link
from within support it brought me to instruction I assume you saw.
Well yes those instructions are correct however to me and I woudl assume most no that is still technically not a gerber viewer.
I'm somewhat new to PADS also but as far as I know
all that "Verify Photo" does is output another gerber (important note) FROM the gerber file you already output and not from the board database.
So in a sence yes it is bringing in the gerber file and outputing another gerber file (hopefully the same) which is checking that the gerber file can be read and this is what it looks like.
However the only means PADS provides to view either gerber file is that "Preview" function with in CAM which is really (to me) more of a print preview function
which is NOT really a useful means to really visually review your gerber files.
So yes those instructions are correct they work as stated however I would never use this method to verify/view gerbers.
But in all honesty the "Preview" function used on the gerbers you are actually outputing it is a nice quick check to see you have all the layers, text etc included in the output
you intended but that is about it, IMHO.
So yes you are techically looking at the gerber output in using "Preview" but I would not call that a gerber viewer by any means.
But what ever floats your boat, if you feel you can verify gerbers looking at that "Preview" fine.
Yes saw yur other post when I finally saw correct
instructions in link I totally never even thought about that function as a gerber viewer, would never have guessed
that is what it was. Expedition really had same kind of deal where you were really just using a sort of plot preview also
which was quite a bit better that this to view but still we never used it for gerber review either. But back then
Expedition (VeriBest) came with a seat of Wise GerbTool.
I am curious-what sorts of things have you guys had issues with?
You know, I have always heard about folks viewing their Gerbers after outputting them, but I never have done this myself.
I have done PCB layouts for 15+ years, and never had an issue, other than stupid little things, like missing moving a REFDES, etc.
Never had problem with anything else.
1. Verify the layers are lined up. PADS makes it very easy to get a layer offset, and that usually makes the fab mad.
2. Review silkcreeen clipping; I'll load a silkscreen layer and a soldermask layer. In Viewmate if you make one layer green and the other red, any spots that are going to get clipped will show up in yellow so they are very esay to see. If I don't find the clipping acceptable I'll go back and rework the silkscreen.
3. Silkscreen/via collisions - you can load the NC Drill file into Viewmate and see if any of the silkscreen is falling on holes.
4. Find out where a tiny D-code accidently got called out that will drive the PCB price up or make it unmanfacturable.
That's what pops off the top of my head.
I see...never had to deal with most of this when I was using PCAD.
I have seen how easy it is in PADS to get the offsets screwed up from plot to plot.
I clear paint from holes myself-I edit the decal in PADS for the individual instance.
Had to do this in PCAD also, but I could graphically modify the part outlines right in the design.
I also have had experiences with trying to find something that I inadvertantly put on the board, but can't see-kind of like the D-code situation that you mentioned.
I have been trying to download the free version of Viewmate, so that i can try it out.
If it is useful, I'll buy a copy.
Had to keep pausing/restarting the download-I could only get 2-3% at a time.
Hope it didn't screw up the install file!
Thanks again for the advice!
Interesting did you go to Pentalogix site to download Viewmate? Or elsewhere?
The only things I would add to issues that come up with output data are:
It seems to help looking at gerber in another environment or so called free viewer of one of the CAM tools a fab house would use.
A. I seem to spot stuff I didn't see in the CAD tool after stairing at it in that tool for too long.
B. I also spot things that are settings or set up related to the gerber output. Especially with planes.
Now you can save settings but when you need somethign different and forget to change something hopefully it gets spotted while reviewing gerber.
What gets output may not have been what you intended becuase you forgot to check off some parameter
maybe for only one of the plane layers etc.
It just seems being in another tool almost makes up for a second set of eyes even if they are still are only your eyes.
Now if PADS did actually provide this "Preview" such that it actually looked like with color and all a CAM seats view fo the data
then it might be usable, (Expedition almost had that) but I still prefer to look at it in another tool anyway for verification.
Yes, I went to Pentalogix to download Viewmate, because it was the first return from my search for “Viewmate”.
I registered, and started the download of the free version, which I will buy if I like it.
But I had to keep pausing and restarting the download, because I would get 2-3% of the file, then the download would stop.
Pausing and restarting numerous times was the only way I could get the whole file.
I hope it isn’t corrupted!
I understand that there are obvious things, like crossing routes, that I need to look for, and I have experience with the “can’t see the forest for the trees” syndrome which occurs after looking at the same layout too long.
I was hoping for some insight into just what other designers look for in their Gerbers, but as I suspected, it is the kind of thing that comes with experience.
I have a decent amount of experience-I have been laying out boards for about 35-40 years, professionally for about 15.
I just always worry about not seeing issues until I get boards.
Everybody probably has the same fear.
I am a perfectionist, that is my burden!
Thanks for your input.
I’ll try not to worry so much!
Have you looked at the ODB++ output and viewing capabilities in the latest versions of PADS? There are quite a few opportunities there:
1. you can switch away from Gerber (very inefficient for manufacturing hand-off) to ODB++ (the vast majority of manufacturers can accept this format and will thank you for it).
2. The PADS software includes the ability to compare the old-style Gerber data to the new ODB++, so you can verify that the ODB++ is the same (or better) in terms of representing your design intentions to the manufacturers.
3. If you want to make an automated analysis of the main DFM problems your manufacturer may encounter, there is a new optional function called "DFMA" in the latest PADS versions. This will allow you to make all the important DFM checks on your design before sending it to the manufacturer.
More information about ODB++ and its benefits can be found at www.odb-sa.com.
Julian Coates (Mentor)
10 years on and off with PADs and I didn't come across that! Anyway, as per some other comments here I agree it doesn't seem that useful anyway. To check gerber files prior to sending for manufacture we have always used GC-Prevue http://www.graphicode.com/GC-Prevue#download . (and when I wanted to make a panel of mixed boards I used the paid version of same which is called GC-PrevuePlus)