Username:
Password:
Save Password
Forgot your Password?

 All Forums
 Help For Easy-PC Users
 PCB Layout
 How to add resist on copper pour area?
Author Previous Topic Topic Next Topic  

rbuck

USA
63 Posts

Posted - 02 Apr 2022 :  04:01:48  Show Profile  Reply with Quote
I have a board with a copper pour area on the entire bottom layer. There will be two brackets that mount this board to a metal chassis. The copper pour area is at ground potential as is the chassis. There is a hole through the board so the brackets can fasten to the board. The bracket is 0.5 in x 0.75 inch.

How do I create a 0.5 x 0.75 inch solder resist pattern that I can place where the bracket will be placed? I need have the entire bracket area to make contact with the copper. I tried creating rectangular pads but when I pour the copper fill it connects the pads to the pour area with 10 mil traces.

I have worked around the problem by creating copper pour areas that span the space between the pads and the main copper pour. I set those copper pour areas as flooded. It works but that is really just a hack.

It would be better to just be able to place a resist area on top of the copper pour at the bracket location.

Edited by - rbuck on 02 Apr 2022 04:03:01

Iain Wilkie

United Kingdom
1011 Posts

Posted - 02 Apr 2022 :  09:11:55  Show Profile  Visit Iain Wilkie's Homepage  Reply with Quote
Simply create the shape of the resist you want clear and place it on the resist mask.

Please note you need to have resist mask layers in your design so if you don't have these you need to add them. Good idea while your about it is to add paste layers as well.

Iain
Go to Top of Page

edrees

United Kingdom
769 Posts

Posted - 02 Apr 2022 :  12:03:00  Show Profile  Visit edrees's Homepage  Reply with Quote
Agree 100% with Iain.

Just remember that the Solder Resist is a "negative" image when you view it with the Solder Resist layer manually added, so instead of "adding" a rectangle you are in-fact "removing" a rectangle of Solder Resist on the actual pcb. It will show correctly as such on the "3D viewer".
Go to Top of Page

rbuck

USA
63 Posts

Posted - 02 Apr 2022 :  17:12:52  Show Profile  Reply with Quote
Ian,

Thanks for the reply. How do I add a resist layer to the design? I have searched and don't see that as an option. I can add paste mask and solder mask, but resist mask is not visible anywhere.

I know they are active because if I plot the board they show up in the Gerber files.
Go to Top of Page

rbuck

USA
63 Posts

Posted - 02 Apr 2022 :  18:30:49  Show Profile  Reply with Quote
Ian, I figured it out. I added a layer named "Bottom Resist" and set the type to Solder Mask. I now see that layer in the Layers dockable bar on the right side.

I created a shape and assigned it to the "Bottom Resist" layer. When I plot the board the resist for the shape shows when I view it in a Gerber Viewer.

What is strange is that in Version 24 the resist layers and paste layers showed up in the Layers dockable bar. The only layers that show up in Version 25 are the copper and silkscreen layers.

edrees, yes, I was aware of the negative aspect.

Thanks for the help guys.
Go to Top of Page

rbuck

USA
63 Posts

Posted - 02 Apr 2022 :  19:43:25  Show Profile  Reply with Quote
I notice one strange thing when adding a resist layer. When I look at it in a Gerber viewer, the added resist layer ignores vias. It treats them as pads. In other words, it creates a non-resist area around the via. When the board is made, the resist will not cover the via, instead it will be plated.

If I look at the default resist layer "Bottom Copper (Resist)", that layer knows the difference between a via and a pad. If I send the default resist Gerber file to the board house the vias will be covered. But the default resist layer does not have my created rectangles resist present.
Go to Top of Page

edrees

United Kingdom
769 Posts

Posted - 02 Apr 2022 :  21:16:36  Show Profile  Visit edrees's Homepage  Reply with Quote
Look at the "properties" of the solder resist layer under Design Tech. You can set the resist "exceptions" for various pads and vias etc. depending on whether you want the vias "tented" with resist (or not).

Also check you have solder resist layers for both Top & Bottom layers and that you have added the rectangle on the correct side.

The plating of the via/pad is determined whether it is a "plated" hole or not, and not by whether its covered by resist or not. Plating is an earlier process than solder resist.

Edited by - edrees on 02 Apr 2022 21:20:10
Go to Top of Page

rbuck

USA
63 Posts

Posted - 03 Apr 2022 :  03:11:29  Show Profile  Reply with Quote
Ed, thanks! That was the solution. Under Layer Types, vias was set to Yes for the Solder Mask layer. Changing it to No applies the resist over the vias.

I guess the default resist layers must be set to No. Apparently there is no visibility into the default resist layers. If there is, I have been unable to find them.
Go to Top of Page

Iain Wilkie

United Kingdom
1011 Posts

Posted - 03 Apr 2022 :  11:23:06  Show Profile  Visit Iain Wilkie's Homepage  Reply with Quote
The great advantage of adding these layers is you can modify them and see the outcome without needing to generate and view gerbers.
Sometimes you need to modify the resist (as in this case) and sometimes the paste mask if for instance you do not want paste on particular pads e.g. edge connectors.
Go to Top of Page

edrees

United Kingdom
769 Posts

Posted - 03 Apr 2022 :  11:33:53  Show Profile  Visit edrees's Homepage  Reply with Quote
quote:
Apparently there is no visibility into the default resist layers. If there is, I have been unable to find them


If you have manually set up both Solder Resist Layers (and (both) Solder Paste Layers if necessary) as Iain has suggested, then you will be able to see each of the Solder Resist layers on the screen as "WYSIWYG" and verify whether your vias are "tented" or not.
Go to Top of Page

rbuck

USA
63 Posts

Posted - 03 Apr 2022 :  19:15:02  Show Profile  Reply with Quote
Thanks Iain and Ed. Going forward I will use this method for all but the most simple boards.

In the past I have had to use a Gerber viewer more times than I liked. Being able to see these layers in the design is a big advantage.

Go to Top of Page
  Previous Topic Topic Next Topic  
Jump To: