I have been using Arial for assembly drawing RefDes and text for years and find no problem doing so.
The Expedition Gerber photoplotter routine will not fill in a filled font like Arial. It will follow the font outline from hint to hint (font geometry handles) but will not fill in the space(s) contained within. So Mentor suggest that you use a stick font so that the finish graphics look the same as your design database. That said, I have been using Arial for photoplotter text as well. By adjusting the line thickness most the the RefDes on the board will not have hollow bodies and it looks good. If the text is too large to be filled in by adjusting the line thickness, then change the font to a VerBest stick font or use an CAM product to do the filling of the hollow areas that appear in Arial.
Since I don't put my Assembly Drawings out to gerbers, I switched to Verdana as my font of choice about a year ago without any issues. For silk, I still use Gerber0
since Ver 2007 (5?) there is a new Group of Fonts vf_xxx, that shows real widths in layout.
Gerber out is ok without any issues.
Advantageous is the minor area consumption of free text in copper areas than with vb0.
To make an assembly drawing for documentation you can take Arial etc. and then make pdf-files with print preview.
To print silkscreen on the Boards you better use the silkscreen layer with e.g. vf_std, you can see all in real proportions.
You have to use the Silkscreen Processor to produce the silkscreen layer; in gerber output processor you must check the Altered Silkscreen Top or Bottom.
This way allows independent outputs for documentation and fabrication.
Cell editor has the two different oprions to do so.
hope it helps
On a slightly different topic, how are you handling text that you do NOT want photoplotted? If you set the line width to "0" and generate silkscreen the value set in "Width options" to "0", the silkscreen generates a 1 th line. I thought 0 th would mean 0 th? I was told on SupportNet that I should put the silkscreen on the pad and then it would be clipped. Any other suggestions that may be more helpful?
I put the silk on a pad and make it small enough that the whole thing gets clipped. I have done it this way for years without any issues
why such circumstances?
Delete all you don´t want to print. You don´t loose anything else.
If you need the names (or outlines) back, simply mark them in place mode and go to >eco >replace cell >(reset on, selected parts on).
Then check the parts in the list and uncheck "keep text attributes during replace".
If you have a sophisticated Library, you simply can use the Silkscreen Generator to select package groups and add them to silkscreen layer.
The rest doesn´appear.
If you haven´t, you can do it in your local library by classing the packages in local cell editor with the appropriate package group.
Guenter, Thanks for the input. I recommended your first solution but it wasn't highly accepted by my user community. I like the idea of processing only selected package groups.
Thanks again for the suggestion.
Great tip!! I guess I have never even noticed that was there until you mentioned it.
All silkscreen items with line width 0 are processed in silkscreen generator with presetted values on the width options.
The other widths are untouched.
Ideally, that was my first option but there seems to be a bug in the software which was the reason for my original post. If the text is set to zero and you set the width option to zero as well, the silk screen generator generates a .001". I opened an SR with Mentor Support a number of months ago, but it was not assiged as a defect.
perhaps there is a little misread.
Outlines and text on silkscreen layer in Layout must be (set to) zero. Then processing with "real" values in the width options of Silkscreen Generator.
The zero setting can be done from library or by hand; checking the width in layout must say "0".
You can´t output gerber with a 0-width. Gerber is used for a real project (drawing copper lines), any output width of 0 is not leading to a real product.
I think "0-width" is not defined for gerber, therefore is gerber output not settable to zero.