GerberX2 export - no assembly layer, bug?

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
dippel59
Posts: 7
Joined: 02 Nov 2018, 05:04

GerberX2 export - no assembly layer, bug?

#1 Post by dippel59 » 20 Mar 2021, 06:41

Hello,

here is a small layout for a step-down-regulator:
- top
- top with top assembly
- mask with paste.

BTW: how I can change order of layers, so top with all traces is visible over top assembly?
TP62260(top)k.jpg
TP62260(top-ass)k.jpg
TP62260(mask+paste)k.jpg
Design check tells me "no error". Also preview of GerberX2-export looks fine.
Then I uploded the zip-archive to Ucamo. They are owner(?) of Gerber-fileformat and call their homepage "reference gerber viewer". I got three messages:
BoardOutline.gbr: Standard attribute '%TF.FileFunction,Profile' is invalid
TopAssembly.gbr: Standard attribute '%TF.FileFunctuion,Drawing,Top' is invalid
TopDimension.gbr: Standard attribute '%TF.FileFunctuion,Drawing,Top' is invalid
And it looks different:
TP62260(Ucamo)k.jpg
I also uploaded at PCBWay. Both homepages don't draw the top assembly-layer.

Is there a bug inside DipTrace?
Do I make something wrong?
If it may be important: DipTrace 4.0 Free on Win10 64bit.

Kind regards
Jürgen
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1739
Joined: 20 Jun 2015, 14:39

Re: GerberX2 export - no assembly layer, bug?

#2 Post by Tomg » 20 Mar 2021, 08:58

Did you include the Board Outline in your Gerber file set?
Tom

dippel59
Posts: 7
Joined: 02 Nov 2018, 05:04

Re: GerberX2 export - no assembly layer, bug?

#3 Post by dippel59 » 20 Mar 2021, 11:16

Yes, a BoardOutline.gbr is inside the zip-archive.

Jürgen

dippel59
Posts: 7
Joined: 02 Nov 2018, 05:04

Re: GerberX2 export - no assembly layer, bug?

#4 Post by dippel59 » 21 Mar 2021, 06:32

Inside BoardOutline.gbr I see a line

%TF.FileFunction,Profile*%

Specification about Gerber files tells me, that "profile" must have a label P or NP.
So DipTrace is producing invalid export?
And what does "edge-plated" mean? A metal cover around the board outline?


Another error is the line    %TF.FileFunction,Drawing,Top*%    inside TopAssembly.gbr - specification only knows
- AssemblyDrawing
- ArrayDrawing
- FabricationDrawing
- OtherDrawing

Tomg
Expert
Posts: 1739
Joined: 20 Jun 2015, 14:39

Re: GerberX2 export - no assembly layer, bug?

#5 Post by Tomg » 21 Mar 2021, 09:50

Would it be possible to post your board file (*.dip) here for others to examine?
Tom

dippel59
Posts: 7
Joined: 02 Nov 2018, 05:04

Re: GerberX2 export - no assembly layer, bug?

#6 Post by dippel59 » 21 Mar 2021, 12:00

Here it is:
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1739
Joined: 20 Jun 2015, 14:39

Re: GerberX2 export - no assembly layer, bug?

#7 Post by Tomg » 21 Mar 2021, 15:02

I noticed that the PCB is far to the left of the Design Area origin, which may or may not be causing possible Gerber translation problems with outside viewers...
fl1.png
As an experiment, try moving the Design Area origin to the lower left corner of the Board Outline as follows to see if it helps...
1) Main menu: View > Define Origin > By Mouse Pointer.
2) Left-click on the lower left corner of the Board Outline.
3) Press softkey [F1] if the Design Area origin is not showing.

You should end up with something like this...
mo1.png
In the meantime I'll continue looking at other possibilities.
You do not have the required permissions to view the files attached to this post.
Tom

Tomg
Expert
Posts: 1739
Joined: 20 Jun 2015, 14:39

Re: GerberX2 export - no assembly layer, bug?

#8 Post by Tomg » 21 Mar 2021, 15:35

It looks like you might want the Top Assembly layer to be copper instead. If so, here's how to do the conversion...
1) Go to the main menu and click on Edit > Edit Selection... to bring up the Edit Selection dialog window.
2) In the Edit Selection dialog window enable [x] Shapes/Pictures, choose Top Assembly in its drop-list and click on OK.
3) Right-click on the edge of one of the selected Top Assembly objects and choose "Properties..." in the context menu to bring up the Shape Properties dialog window.
4) In the Shape Properties dialog window choose "Signal" in the Type: drop-list and click on OK.
"...what does "edge-plated" mean?..."
It probably means you have copper too close to the edge of the board. During the fabrication process the board will be cut with a shear and if the copper is too close to the board edge, that copper could be smeared down the side of the board resulting in shorts to other layers that may also have copper all the way to the edge of the board. The board on the right uses manually-placed copper pours and a few traces of various widths, instead of standard filled-polygon drawing objects. It also employs the DipTrace default setting for edge clearance...
cmp2.png
You do not have the required permissions to view the files attached to this post.
Last edited by Tomg on 22 Mar 2021, 07:13, edited 1 time in total.
Tom

dippel59
Posts: 7
Joined: 02 Nov 2018, 05:04

Re: GerberX2 export - no assembly layer, bug?

#9 Post by dippel59 » 22 Mar 2021, 02:21

Tomg wrote:
21 Mar 2021, 15:35
It looks like you might want the Top Assembly layer to be copper instead. If so, here's how to do the conversion...
Yes, that's what I want to do.
During my first try I placed filled shapes directly to "top" and got a lot of errors from design rule check.

So what is the reason for a "top assembly"-layer?
What does an experienced user place on this layer and what normally happens with this layer during pcb production?


I made layout large to have clearance, moved origin to left lower corner and moved shapes from top assembly to signal. So her is the result:
Ucamo.jpg

The result of PCBway is what I expected:
PCBway.jpg
So I don't know, if Ucamo is really the reference ...

Jürgen
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1739
Joined: 20 Jun 2015, 14:39

Re: GerberX2 export - no assembly layer, bug?

#10 Post by Tomg » 22 Mar 2021, 07:22

...So what is the reason for a "top assembly"-layer?
What does an experienced user place on this layer and what normally happens with this layer during pcb production?...
The assembly layer is for documentation. Its main purpose is to show how to load components onto the board (placement, orientation, etc). Even though you know where everything is supposed to go, if the blank boards are sent to an assembly house they will need the assembly layer documentation in order to load them as you intended.

If you are going to load the boards yourself then you do not need to include the assembly layer in the Gerber file set that is destined for the board house.

If it makes you feel any better, I get the same "invalid" message from the free Ucamco viewer. It is possible that a minor flaw exists in the DipTrace Gerber generator. I really do not know. Maybe we could get Alex or Serg to look into this to see if the problem is with Ucamco or if there is a problem with DipTrace itself...
ucamco_bo2.png
You do not have the required permissions to view the files attached to this post.
Tom

Post Reply