Kinds of apertures in System DXP2004

[Delsian]

gerbt00l

Suddenly I found strange thing. System DXP2004, I made Gerber files for manufacturer. QFP chips placed with step of 90 degrees, turn out with normal rectangular apertures, each leg is described by one aperture.

On a new design I has put one QFP under a corner of 45 degrees. I take out in Gerber and send a file to manufacturer, and it returns to me Gerber back - because I made wrong apertures.
I look at this microcircuit closely in Camtastic - yes, each pad not solid, and consist of several lines in width 5mils. I turn a QFP chip on 90 degrees - pads solid. I turn on 45 - again lines. Well, we admit, that Pr0tel does not know that apertures can turn not only under a right angle (though it is rather strange for such powerful package) and replaces them by lines.
Already even the manufacturer has agreed to draw pads by lines, only requirement - the width of a line should not be less than 5mils. But I cannot find at all where to change this width!

Who with such collided, how such to treat? On protel.com in knowledge base anything such it is not mentioned

 

[House_Cat]

Re: DXP2oo4 and apertures

There are two kinds of apertures - draw and flash. Both are legitimate types of apertures.

A draw aperture is what you saw made up of 5mil lines. Draw apertures use short segments of lines to fill in a shape such as a rectangle, octagonal pads, etc.

A flash aperture is defined as a solid shape. This is what you saw when you rotated the pad to a 90deg position.

There is nothing wrong with your Gerber files - you have an ignorant manufacturer. His CAM software can't properly interpret the Pr0tel D-Codes. Instead of trying to fix his problem, he dumped the files back to you.

D-Code tables are different from one EDA program to another. The PCB fabricator has to understand what format he is working with, and make sure that he reads the data into his CAM software properly.

You have two options.

1-Find a better PCB fab.
2-Read your Gerber files into a third party Gerber editor, such as CAM35O or GERBT00L and write them back in a format your existing fab knows how to use.

I recommend you find a more competent PCB fab.

The 5mil draw cannot be changed withoud degrading the quality of the pad. The size of the line is determined by the size of the pad, and the resolution you specify in the "match tolerance" option of the Gerber setup window. The equipment your PCB fab is using must be antique if they can't handle 5mil lines - most fabs I have dealt with can handle D-CODE lines down to 1mil. Remember that these lines aren't actually put on the circuit board, they are only used to expose film or a mask to make the circuit board. It's like filling in a box by scribling a fine pencil line inside the outline.

 

[Delsian]

Re: DXP2oo4 and apertures

Thanks for teory, it's very interesting.

You have two options.

1-Find a better PCB fab.

I don't know another fab with such cheap cost of prototyping, as https://run.to/pcb
Additionaly, they located near my country, so shipping will be also very cheap and fast.

2-Read your Gerber files into a third party Gerber editor, such as CAM35O or GERBT00L and write them back in a format your existing fab knows how to use.

No, when I examine Protel's CAM output - it contains also lines instead of pads. You mean I must change pads in CAM manually?

In local newsgroup one man gave me a piece of good advice - I simply changed pads from rectangular form to round, and solve problem with pads. Now I'll wait for fabricated boards to check if QFP will fit to new pads

Anyway, thank you for answer.

 

[House_Cat]

Re: DXP2oo4 and apertures

I guess I didn't explain very well.

You have lines in CAMTASTIC because you told Pr0tel DXP it was OK to use "draw" apertures, or both "flash and draw". The lines in Camtasitc are normal for "draw" apertures. There is nothing wrong with your Gerber file.

To remove "draw" apertures, you can either tell Pr0tel to use only "flash" apertures, or you can load your Gerber file into a third party Gerber editor, and save the file from there with only "flash" apertures. Not all Gerber editors can recognize and convert a drawn aperture - it takes one of the high end tools to do that.

Once again - there is nothing wrong with having shapes in a Gerber file that are made up of short lines. Those shapes are called "draw apertures". You shouldn't have compromised your design just to satisfy the fab.