Please contact CAM350 supplier for possible solution. Also you can use ODB++ export and is is a single, intelligent file that is a better format then Gerber.
i use ViewMate all the time with no issues. Do you have an offset defined on some or all layers? Attaching photos of the issue may help.
Gerber output justification is based on the extents of each gerber file, so when you use Bottom Left, it could be different for every layer. The exception is when you use the Offset justification. The offset is based on the Board origin, and it needs to be the same for every layer, including the drill file, in order to align all of the files. It also should be large enough to place all of the gerber files in the positive quadrant.
So when looking at your PCB, zoom out so you can see everything, and place your cursor so it's below and to the left of those extents. That is the minimum offset you need. Round up to whole numbers to make it easier to enter, since you need to do that for every CAM file. So if the cursor is at -1300 mils for X and -2400 mils for Y, use 2000 and 3000 for the offsets.
Thanks for above answer.but my question is i have the board file which has board origin in center only.i Generated Gerber (Justification is Bottom left only).
After import the gerber it should be located in origin of cam file right.For example,i imported the gerber in viewmate here i attached in image file.
I have just tried your setup, the reason why it is not aligning the origin of PADS and Viewmate is that the gerber data will go out of the co-ordinate in to the negative plane region of your gerber sheet, since it took the extremes of your gerber data and aligned with the extremes of the gerber sheet.
you can go through the preview in CAM section before exporting gerbers to see how exactly your setting effect the location of the data.
best practice is to keep the origin in bottom left corner , and use "offset" as the justtification in CAM setup as david.ricketts suggested
Thanks for your reply.Evern i set the origin in bottom left also i am getting issue
Delete the text and try once
I may be stating the obvious:
- Gerber format doesn't support negative coordinates. PADS will send up a warning that it is adjusting the offset to keep all coordinates positive. With your board origin in the center of the board you have negative coordinates, so you or the tool need to define an offset.
- If you are using justification and letting the tool set the offset, you really need a common shape (like a title block) around EVERYTHING on every Gerber layer/file. There needs to be a common shape to align with. I use OFFSET and manually set the offset the same for every Gerber file.
Thanks for your reply.i am using positive co ordinates only
With your PADS origin in the center of the board as shown on 6/26/15 you are indeed using negative coordinates for anything to the left or below the origin.
Why do you want your PADS origin and your Gerber origin at the same spot? As long as all the Gerber files line up then your Gerber origin is correct for the fab house.
Generally,origin is General Co-oridnate for all the tool right.But i could not understand why viewmate not support the PADS Gerber origin location.for example,autocad dxf origin support with all the tool origin location even it support PADS also right ?? like that i could not understand why it is not support the Gerber ??
Interesting. I looked up the Gerber standard (you can Google it) and see it does support negative coordinates. Only PADS does not support negative coordinates in the Gerber output. That's odd.