topic Re: Closing small gaps in poured ground layer in Fusion Electronics Forum

Closing small gaps in poured ground layer

ilia.vitsnudel — Tue, 07 Jan 2025 15:57:34 GMT

Hello, I would like to close small gaps that have been left after Polygon pouring for the ground layer or make some small additions to improve the shape. I have tried to reuse Polygon pour command, but it seems to generate an empty dashed polygon that doesn't seem to add an additional ground.

I am attaching an example of what I would like to achieve.

Thank you,

Ilia Vitsnudel

Re: Closing small gaps in poured ground layer

Evert_2N3055 — Tue, 07 Jan 2025 19:12:59 GMT

Looks like you have some underlying traces that makes the poor look strange because they stick out a bit. Click on the spot you want to edit, toggle with a right click until the trace is highlighted and move or delelte it.

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Tue, 07 Jan 2025 20:22:11 GMT

Yes, this looks strange because I was using small traces in order to make
the poor look better. I however need to be able to add additional pour to
the grounds to make RF Grounded Coplanar Waveguide microstrip lines to look
smoother and better. By the way, I also saw that the gaps around the RF
lines are drawn as piecewise linear segments (and not smooth curved lines)
which also somewhat breaks the definition of the RF GCPW lines when being
unpoured automatically around the RF lines.

Thanks,
Ilia

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Wed, 08 Jan 2025 19:07:21 GMT

@jorge_garcia

Jorge, do you have any suggestions on how to pour small ground polygons in addition to the big ground polygon pour. I need this to manually overwrite the automatic pour to fix few discrepancies. If I use additional polygon pour I am getting wide dashed outlines without internal fill.

Thank you,

Ilia

Re: Closing small gaps in poured ground layer

jorge_garcia — Thu, 09 Jan 2025 18:48:31 GMT

Hello @ilia.vitsnudel,

I hope you're doing well. If the polygon is smaller than a certain point it won't fill. For what you are trying to do it might be better adjust the larger polygon outline so that is fills better. If this is not an option then the best thing is to use small short trace segments to fill the polygon outline.

I don't know what type of frequencies you are dealing with but this might be a case of diminishing returns and it might not be worth the effort to round out that polygon.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Thu, 09 Jan 2025 19:26:42 GMT

Thank you Jorge,

The working frequency is 6GHz, so every small discrepancy generates discontinuity in signal propagation. I would like to have well defined gaps. I have tried tried to use small traces to fix the polygon segments, but I can't place traces anywhere I want. They have to originate from the pad and end at a wire. Besides if I have placed a wire I can't place another one emanating from the same pad.

I have tried to use bigger polygons and I still getting the dashed polygon outline.

Do you thin it is somehow possible to export the ground layer to Fusion, patch it there and then bring back to board?

Re: Closing small gaps in poured ground layer

jorge_garcia — Thu, 09 Jan 2025 20:03:18 GMT

Hello @ilia.vitsnudel,

You can use the line command to freely place traces wherever you might need them. Just make sure to give them the appropriate signal name.

The mechanical modeling environment of Fusion won't help in this scenario. The polygon is calculated dynamically and no editing done elsewhere will really change it. I'm sorry you are running into this, I'm documenting all of this to build the case for getting it improved.

Best Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Thu, 09 Jan 2025 22:05:04 GMT

Thank you, Jorge.

It might actually work if I use line and arc commands together. I did a little experiment and I am getting close. I will write some code tomorrow to actually calculate the desired end points and sizes for the arcs and will let you know. Is there a possibility to add lines/arcs programmatically?

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Thu, 09 Jan 2025 22:43:04 GMT

Hi @ilia.vitsnudel,

Regarding your question: "Is there a possibility to add lines/arcs programmatically?" - the answer is no. This is not possible because the polygon clipping algorithms we use don't support arcs. All arcs are converted to line approximations. What we can do is to make the arcs approximations tolerance smaller (smoother line approximations). This will not completely clear the 8dB loss you are seeing but it could reduce it drastically. The draw back with this is that the copper pour calculations could become slower. We already have a ticket to add support for specifing the polygon arc's tolerance per copper pour.

Kind Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Thu, 09 Jan 2025 22:59:40 GMT

Thank you. Is this arc tolerance approximation is something that I can do or should it be done by you?

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Thu, 09 Jan 2025 23:43:01 GMT

Hi @ilia.vitsnudel,

We need to add support for this because right now it is hardcoded and this is the issue. We'll try to add support for this as soon as we can.

I hope this helps.

Kind Regards,

Re: Closing small gaps in poured ground layer

jorge_garcia — Fri, 10 Jan 2025 19:13:06 GMT

Hello @ilia.vitsnudel ,

I hope you're doing well. Just to answer your question, it is possible to programatically draw in lines and arc see the line and arc commands here:

https://help.autodesk.com/view/fusion360/ENU/?guid=ECD-CLI-L

Line command documentation here

https://help.autodesk.com/view/fusion360/ENU/?guid=ECD-CLI-A

Arc command documentation here

Let me know if there's anything else I can do for you.

Best Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Fri, 10 Jan 2025 22:51:40 GMT

Thank you Jorge.

Very useful, I was able to draw a perfect anti pad around the through hole
pads of the antenna feeding point by using a combination of arcs and lines
(actually lines were drawn by arcs too). Now there are two questions in my
opinion:
1. In order to use the arcs I had to define slightly bigger than needed
Wire-to-Pad clearance so the piecewise linear approximations of the circle
will be later patched by adding an arc with a proper diameter. The question
is can I define rules so only those specific through hole pads which feed
the antenna will be affected by the rule without affecting other pads that
have to be at another distance?
2. If I follow your suggestion of manually routing the ground traces along
the Grounded Coplanar Waveguide RF lines so as to obtain smooth ground
lines then ground polygon pouring with its piecewise linear approximation
will sneak to the gaps and break nicely outlined manual ground lines again.

I appreciate very much your help,
Thank you again,
Ilia

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Sat, 11 Jan 2025 00:47:00 GMT

Hi @ilia.vitsnudel,

Regarding question: "1. In order to use the arcs I had to define slightly bigger than needed Wire-to-Pad clearance so the piecewise linear approximations of the circle will be later patched by adding an arc with a proper diameter. The question is can I define rules so only those specific through hole pads which feed the antenna will be affected by the rule without affecting other pads that have to be at another distance?" - you can do this by using a scope like: Is Pad and In Component('Your Anntena Component) and In Signal('Signal Name'). You need to add one rule for each pad if the pads connect to different signals or the pads are in different components. These rules should have higher priority (lower number) then any other rules so you need to move thema at the top of the copper clearance rules list. If you have SMDs then replace Is Pad scope with Is Smd.

I hope this helps.

Kind Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Sat, 11 Jan 2025 20:16:40 GMT

Thank you Constantin,

I think you are right that it might be done by properly defining Custom
Design Rules.
However, I am struggling implementing this and I wonder if you can help me.
My starting point is shown in the PieceWise1.jpg image. The desired gap on
the Grounded CoplanarWaveguide is 8.01 mil and the Anti-pad release is
8.68504 mil, both exactly as it should be when specified by Wire-Wire and
Wire-Pad clearances.
The problem is however that the Anti-pad is represented by piecewise linear
approximation instead of a smooth circle.
So as the first step I am increasing Wire-Pad clearance to 12 mil as to
allow nice covering of the piecewise linear approximation by an additional
wide arc with to get desired Anti-Pad radius.
For this I am changing the Wire-Pad design rule as shown in PieceWise2.jpg
image.
Now, I am drawing a wide arc (defined as DGND signal, same as the poured
DGND polygon). The parameters of the arc are shown in the PieceWise3.jpg
image.
(I am using the following command:
ARC 'DGND' CW FLAT (1997.1477 1798.3743) (1995.6286 1745.0258) (1969.7139
1770.9405) 14;
The problem is that the width of the arc as I calculated it in order to get
the desired Anti-pad release should be 14 mil, but in reality I can't get
it wider than 8 mil, probably because of the Wire-Pad rule. So, I have
tried to define a custom design rule for Wire-Pad, but I can't get it
working, it doesn't seem to make the arc wider than 8 mil. My definitions
for the custom design rule are shown in the same PieceWise3.jpg image. I am
certain that I have not defined the rule properly and would like to ask you
to take a look at it and hopefully make it work.

I think I will also have to add small lines (again by using the arc
command) to fill small gaps that will remain after applying the wide
semicircular arc, but I think once I will understand how to make custom
design rules I will be able to do it.

Thanks for your cooperation and help,
Ilia

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Sun, 12 Jan 2025 22:01:09 GMT

Hi @ilia.vitsnudel Ilia,

There is one behaviour that might interfere with the binary custom design rules (copper clearance) and that is that we use the maximum clearance value between the applicable General Rule (wire-pad in this case) and the best applicable cutom coper clearance rule. This implies that in order for the custom rules to work the General rule value must have the smallest of all the copper clearance rules values general and user defined (custom rules). I guess that this might be what happens in your case.

I think that you forgot to attach the pictures described in your respones so if you can attach them that would help me get a better idea of whta might be happening in this case.

I hope this helps.

Kind Regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Mon, 13 Jan 2025 05:14:17 GMT

Sorry about the images. Here they are.

Thanks,

Ilia

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Mon, 13 Jan 2025 05:36:54 GMT

Hi @ilia.vitsnudel Ilia,

Thanks for sending the snapshots. I had a look at your custom copper clearance rule and the scope is not correct. The Object 1 Scope should be: 'Is Pad and In Component = SENS_A1:SEN3 and In Signal = DGND', and Object 2 Scope shoul be: 'Is Pad and In Component = SENS_A1:SEN3 and In Signal = OtherSignal' (very similar, so the rule works for pads in the selected component and for different signals). You can add similar rules if you need to check against pads in other components or other signals.

Please keep in mind that it is good practice to create as few custom rules as possible because the more rules you add the slower the DRC check will be. You can always disable rules so they don't impact the DRC check.

I hope this helps. Please et me know how you go with this.

Kind regards,

Re: Closing small gaps in poured ground layer

ilia.vitsnudel — Mon, 13 Jan 2025 08:20:46 GMT

Thank you,

It is still not clear to me how to define the rule. Basically, as the first object I would like to define a pad, with the following scope options: IsPad and InComponent: SENS_A1:SENS3

and the second scope would be the Ground signal: InSignal: DGND

What was the purpose of adding additional InSignal: DGND in the first scope that you have mentioned and why again I should put IsPad and InComponent = SENS_A1:SEN3 in the second scope? And what is the meaning of the InSignal = "OtherSignal"?

At the end I would like to define a minimum distance between the specific Pad belonging to SENS_A1:SENS3 component and the Wire (arc) which is DGND.

Ilia

Re: Closing small gaps in poured ground layer

constantin.popescuXD3CL — Mon, 13 Jan 2025 19:54:29 GMT

Hi @ilia.vitsnudel,

Regarding this questions: "At the end I would like to define a minimum distance between the specific Pad belonging to SENS_A1:SENS3 component and the Wire (arc) which is DGND." - then the scopes should be like:

Object 1: Is Pad and In Component(SENS_A1:SENS3)

Object 2: Object Type = Wire and In Signal(DGND)

This should do what you need.

Kind Regards,