| Author |
 Topic  |
|
|
markpsu
USA
67 Posts |
 Posted - 03 Jul 2020 : 17:07:39
|
I have a 2nd mask layer that has additional mask over (critical) small areas of the PCB. The mask on this layer is drawn by me over traces and is not in "normal" areas like over via's etc.
Since I've drawn this the polarity is reversed, so when exporting to gerber files the mask shows up opposite to where the board house would expect. Is there somewhere way I can invert the mask layer? Checking the export and layer options I didn't find it.
|
|
|
edrees
United Kingdom
766 Posts |
Posted - 03 Jul 2020 : 17:30:16
|
I think you can only have one solder mask on each layer. Why not use the original solder mask layer to "paint" the special areas in? Add solder resist mask to your "Layers" stack so WYSIWYG display in pcb editor.
Not exactly sure what your definitions of "mask" and "polarity" refer to, but I suspect that your "second" mask layer is on the other side of the pcb. Check your Des. Tech. =>Layers stack. |
Edited by - edrees on 03 Jul 2020 17:32:42 |
 |
|
|
markpsu
USA
67 Posts |
Posted - 06 Jul 2020 : 21:13:42
|
I have the 2 mask layers as normal and then another layer on top of the top solder mask layer. This is because we need some areas to have additional mask thickness to prevent dielectric breakdown. So 2nd layer means another run on the same layer of mask.
Really this info probably doesn't matter. I want to be able to reverse the mask layer when plotting to Gerbers so it's no longer negative.
I'm not sure what WYSIWYG display is referring to?
|
|
|
|
edrees
United Kingdom
766 Posts |
Posted - 07 Jul 2020 : 00:16:25
|
I now think I have a better understanding of your issue.
1)EasyPC will only allow 1 solder resist mask on the Top (or Bottom) layer.
2) The Solder Resist Mask by default is a negative plot. If you draw a filled rectangle on the Solder Resist layer it will be clear of Solder Resist,- which is what you are seeing (correctly)!
3)WYSIWYG=> What You See Is What You Get.
Whatever solution you use, you will have to make it 100% clear to your pcb manufacturer what you want as the solution is totally unconventional. I'm not even sure if the second solder resist will stick to the first layer without eventually delaminating.
4)What wrong with asking your manufacturer to print two layers (identical) of Solder Resist? That way you get an uniform double thickness everywhere, but so what?
5)Because of 1) and 2) you could create a new "Special Effects" top layer called "TopSolderResist2". Draw in the areas you want and plot the Gerbers making sure you tell your manufacturer that TopSolderResist2 is a POSITIVE plot.The layer stack will be correct. The Gerber Plot Settings=>Layers=>Positive or Negative Plot will not work for Special Effect |layers.
6)There's possibly another method to "cheat" EasyPC by drawing the extra layer in an unused inner copper layer (set as a Powerplane) called TopSolderResist2 and subsequently changing the Gerber plot settings to create the negative plot. But the layer stack will be incorrect.
|
Edited by - edrees on 07 Jul 2020 09:11:45 |
|
|
|
markpsu
USA
67 Posts |
Posted - 07 Jul 2020 : 13:28:04
|
edrees, I believe you described my issue well...its certainly "unconventional" as usual. I have my answer it seems I can't toggle between -/+ mask layers.
The reason for selective mask thickness is because we have both high voltage and RF. So, adding more mask in the RF portion of the board will change performance. |
|
|
|
edrees
United Kingdom
766 Posts |
Posted - 07 Jul 2020 : 13:45:53
|
Yes, by design a solder resist layer is a negative plot and you are drawing in special areas in positive mode.
You can't have a "double thickness" Gerber layer, -it has to be one layer on top of another. By using the Special Effects layer you can draw your special areas in positive mode, but the Photoplotter must reverse this. Using an inner copper layer (and making it a Powerplane allows you to reverse the plot in the Gerber Plotting Dialogue so the Photoplotter doesn't have to do it. But the PCB manufacturer must be aware of what you are trying to achieve as the Inner Copper Layer has now become the 2nd Top Layer solder Resist.
quote:
I have a 2nd mask layer that has additional mask over (critical) small areas of the PCB. The mask on this layer is drawn by me over traces and is not in "normal" areas like over via's etc.
This is what confused me, how can you have an additional 2nd mask layer, - Easy PC doesn't allow it?
|
|
|
|
edrees
United Kingdom
766 Posts |
Posted - 08 Jul 2020 : 09:59:05
|
There is another way assuming that you are happy with a "Pads Only" solder mask for your normal stuff.
Create a new solder resist mask layer named SolderResist2. Disable (i.e. "No" to all) all the exceptions in the Design Tech, Layers Type Solder Mask table. (not sure if this step really makes any difference).
Flood (filled shape) the pcb with SolderResist2 and use "cutouts" in SolderResist2 layer to place the additional solder resist in the special areas you want.
When plotting manually create a SolderResist1 layer Plot using "Pads Only" plot, and make sure you also have a SolderResist2 Plot enabled.
Now the Gerbers will look as you expected but you will still have to clearly explain everything to your pcb manufacturer!
|
|
|
|
markpsu
USA
67 Posts |
Posted - 09 Jul 2020 : 18:32:09
|
| I was able to trick it into allowing 2 mask layers, I have top and bottom mask layer types and then have a top & bottom type on the top 2 mask layers, so I guess that's why it worked. Then I ended up just drawing the (complicated) shapes where I didn't want the mask. |
|
|
|
edrees
United Kingdom
766 Posts |
Posted - 10 Jul 2020 : 09:34:15
|
Mark,
quote:
I was able to trick it into allowing 2 mask layers, I have top and bottom mask layer types and then have a top & bottom type on the top 2 mask layers
-that's totally thrown me now! |
|
|
| |
Topic |
|
Changing polarity of a mask layer