(Allegro) Etch & Gerber

Hi!
I've switched from Layout to Allegro 16.3 some time ago, but until now I had sent no board to an external manufacturer.
Now that I sent the first board I'm facing a problem and I had no idea how to solve it, so I hope in your help :smile:

With Layout, gerbers were made of lines: from connections to copper pours. Pours were made of a set of lines without space between them to create a copper plane. Simple.
Now, with Allegro, I can create an etch filled as solid or as hatched. In the first case, in the gerber I have a new element, made as a polygon, and placed on a sort of "sub-layer": if I open the gerber file with a program like GC-Prevue I can see these different sublayers where all polygons are placed. This kind of files are not accepted by the manufacturer, so I had to find a solution.
The only way I was able to find was to change all etches from solid to hatched, eliminating the presence of sublayers inside the gerber, but then I had a new problem: Allegro doesn't allow me to set zero space between lines in the hatch, so I always have some void space inside the plane. Besides, it looks like that hatched shapes can't be dynamic, and it's quite annoying...

So, my questions are:
- is it any way to tell Allegro to create gerbers without this sort of "sublayers"?
- is it any way to tell Allegro to avoid the use of polygons inside gerbers?
- is it any way to create an etch "Layout style", filled and hatched?

If my explication is not clear (a distinct possibility...), I can attach some picture to better explain what I mean.

Thanks for any suggestion!

Hi
I'm not work with layout. But I know Allegro.
In Allegro, we can create dynamic etch by using shape and set that as dynamic.

Well yes, I know, but that was not the point.
My problem is at the moment of the creation of the gerber: the company where I send PCB to be manufactured doesn't want etches made of polygons instead of lines.
So I need to switch from a solid fill to a hatched fill, but hatched is... not solid, of course.
So the basic question is: how can I tell to Allegro to create gerber without using polygons?

The outline fill commands G36/G37 are genuine RS-274X (extended gerber) and should be in fact handled by PCB manufacturers. But I'm rather sure, that Allegro has postprocess options to selectively disable extended gerber features like arcs or filled outlines. Did you read the manual thoroughly?

FvM said:

The outline fill commands G36/G37 are genuine RS-274X (extended gerber) and should be in fact handled by PCB manufacturers. But I'm rather sure, that Allegro has postprocess options to selectively disable extended gerber features like arcs or filled outlines. Did you read the manual thoroughly?

Click to expand...

Ehm... I have not been supplied of any manual...
I read the Orcad PCB design book, really well done, but it doesn't say anything about disabling selective the extended gerber features.
I've spent some time looking in program configuration but I was unable to find anything like that.

I'm not using Allegro, but I see that Allegro User's manual, which is comprised of several documents has a seperate book Preparing Manufacturing Data. You should particularly observe the chapter Generating Artwork. It talks about different plotter devices, that can be used. A Gerber 4x00 device should provide plotted polygon fills.

The document file is algroman.pdf, by the way.

I think, there's a problem, that tools like Cadence Allegro are dedicated to professional Layouters, that are spending much time with PCB design and preferably participated in a product training. The fact, that you even don't know about product manuals suggests, that you are rather a casual layouter.

I will give a look at that manual, thanks for the suggestion ;-)
I'm not a so casual layouter really, I've been doing circuits in the last ten years, first as hobby and than for work. I've always been using Layout but in the last year in the new job I had to switch to allegro and they just gave me the program telling me to learn it, so I had to learn it by myself. I have already done six board in the last months with Allegro, but one had no etch, another was manufactured with the machine we have, etc, so this one is the first we send outside and it's the first time I have this kind of problem.

I guess, the major part of CAD tool operation can be learned interactively, without reading a manual. But it's reasonable to get an overview of the available documentation when starting a new tool.

I'm still wondering why your PCB manufacturer can't read filled polygons in RS-274X. I can only imagine two explanations
- he's using a recent photplotter but his software doesn't really support extended gerber
- he has an old vector photoplotter from the 80th

FvM said:

I guess, the major part of CAD tool operation can be learned interactively, without reading a manual. But it's reasonable to get an overview of the available documentation when starting a new tool.

I'm still wondering why your PCB manufacturer can't read filled polygons in RS-274X. I can only imagine two explanations
- he's using a recent photplotter but his software doesn't really support extended gerber
- he has an old vector photoplotter from the 80th

Click to expand...

They produce PCB with milling machines, not with photoplotter.
From what I've been able to understand, I guess -because they were not so clear- that the problem is not the use of polygons, even if they claim that polygons gives more problem at the moment of processing the gerber, but the fact that each gerber layer is made of various sub-layer when polygons are used. I suppose is some kind of software issue, not a limitation of the production process. An alternative of finding a way to create gerber without polygons is to import gerber file in some CAM program, convert them to a single layer gerber and then export again.

I assume that it's simply a software limitation of not fully supporting extended gerber, most likely with the filled polygons feature. In this case, you would need to "fill" (hatch) it in a cad tool.

I saw, that the filled polygon out of Allegro can also involve negative features, e.g. for an isolated pad in a copper pour. They appear as a "c" (composite) layer in GCPrevue. In this case, merging of sublayers won't be possible without removing the isolation. If you only have "+" (positive) sublayers, you can merge them by removing repeated %LPD% statements from the gerber file.

But as said, the legacy Gerber4200 photoplotter definition of Allegro should be able to plot these structures.