Copper Pour DFM Error

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
bixelps
Posts: 8
Joined: 15 Aug 2011, 16:31

Copper Pour DFM Error

#1 Post by bixelps » 17 May 2019, 16:12

Sierra Circuits sent me a DFM report on our design which included an error I am not sure how to resolve. In this error a copper pour surrounds some features. In between some features it attempts to join the pour together again but does not quite make it. The result is a little sliver of gap which is too small of a feature to pass the DFM. I know I can move things around to resolve this particular one but there are a lot of these issues in the design and I want to know if there is any pour property in diptace I can use to prevent diptrace from creating such small gaps?
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1325
Joined: 20 Jun 2015, 14:39

Re: Copper Pour DFM Error

#2 Post by Tomg » 17 May 2019, 17:57

Have you tried reducing the Line Width and Line Spacing values located under the Pouring tab in the Copper Pour Properties dialog window?
Tom

bixelps
Posts: 8
Joined: 15 Aug 2011, 16:31

Re: Copper Pour DFM Error

#3 Post by bixelps » 18 May 2019, 10:46

Thanks for the response. I have played with these settings and they do have an impact on these features. But it seems to solve some issues and possibly create similar problems elsewhere on the layout. My big problem with these two settings is there does not seem to be any documentation about what they do or how to use them. I am a novice so this is an issue for me. I fear to adjust settings which I do not understand.

Where can I learn about these settings and how to set them?
Last edited by bixelps on 19 May 2019, 08:50, edited 1 time in total.

Tomg
Expert
Posts: 1325
Joined: 20 Jun 2015, 14:39

Re: Copper Pour DFM Error

#4 Post by Tomg » 18 May 2019, 12:48

1) In the Main Menu click on Help and select PCB Layout Help in the drop-down menu to bring up the PCB Layout Help window.
2) In the PCB Layout Help window click on the [Contents] tab and navigate down through [+]PCB Layout > [+]Objects > [?]Copper pour to bring up the Copper pour information window.

There is a tutorial that is accessible from within the program (Help > DipTrace Tutorial) and on the DipTrace website here https://diptrace.com/books/tutorial.pdf where you can find more detail regarding copper pours in section 2.11 which starts near the bottom of page 65 (pdf page 66).
Tom

bixelps
Posts: 8
Joined: 15 Aug 2011, 16:31

Re: Copper Pour DFM Error

#5 Post by bixelps » 19 May 2019, 08:49

Again thanks for the responses here but I have not yet learned much.

The MainMenus->Help->PCB Layout help says:
"Line Width – size of the lines forming the copper pour. It is one of the basic copper pour parameters."
My pour is a solid copper pour. How does "line width" work into a solid pour. I am not thinking a solid pour has any lines so this setting should have no meaning. I acknowledge that it does do something. But I cannot understand what it does in the case of a solid copper pour.

The tutorial is completely devoid of information on this subject (other than it mentions the settings exist) although it would be nice is it was covered.
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1325
Joined: 20 Jun 2015, 14:39

Re: Copper Pour DFM Error

#6 Post by Tomg » 19 May 2019, 20:21

If a PCB has a solid copper pour on the top copper layer and a Gerber file is generated for that layer and then that same Gerber file is imported into the top copper layer of a new PCB layout, you will notice that the newly-imported "solid" copper pour will be made up of multiple parallel lines along with short angled polylines (for edges) that are in contact with each other. (If you try this, you'll have to disable Real-time DRC before importing so as not to generate a zillion DRC errors.) I believe this is the way a board house will see a "solid" copper pour because that is probably how it is defined in the Gerber file. However, I can't say this with any certainty because my knowledge of the Gerber file format is practically non-existent.

The reason a solid copper pour is not rendered in precisely the same manner within the Design Area of the PCB Layout editor (you are unable to see its individual lines) is because there needs to be a convenient way to give it the desired shape, location and properties; so you are basically dealing with defining its outline. It is my belief that the solid copper pour you see in the Design Area is actually an excellent approximation of what will be generated by the Gerber exporter for the manufacturer, so any visible small, unwanted gaps are to be taken seriously.

Choosing a smaller Line Width during solid copper pour creation in the Design Area will allow finer detail giving you a better chance of closing those small, unwanted gaps. Be aware that a smaller Line Width might also come with the possibility of longer rendering times when generating or updating all copper pours; especially in larger and/or more complicated designs. As an experiment, try a copper pour Line Width of 0.1mm (4mils or 0.004") to see if things improve. You can always return to the original setting. Just make sure the copper pours are updated after implementing any changes.

p.s. In figure 20 of your first post there is the possibility that not enough room exists to accommodate the narrowest of copper pour lines to close the gap while still obeying clearance and minimum width rules. Also, the actual location of adjacent copper pour lines (not individually visible in the Design Area) might be offset just enough to prevent any of them from crossing through. I am unable to discern the actual size of the voids/holes/pads/gaps in your screenshot.

Here is an example of how one solid copper pour has been automatically constructed by DipTrace...
pour_py.jpg
pour_pr.jpg
pour_al.jpg
You do not have the required permissions to view the files attached to this post.
Last edited by Tomg on 20 May 2019, 10:01, edited 1 time in total.
Tom

Alex
Technical Support
Posts: 3067
Joined: 14 Jun 2010, 06:43

Re: Copper Pour DFM Error

#7 Post by Alex » 20 May 2019, 09:15

Decreasing line width makes copper pours smoother. The drawback is size of output file. Very thin lines are impossible to produce.
Line spacing is not used for solid pouring ( it makes sense for pouring by lines and hatching).

Post Reply