Author Topic: Solder resist problem  (Read 1974 times)

0 Members and 1 Guest are viewing this topic.

Offline pmaggi

  • Contributor
  • Posts: 19
  • Country: uy
Solder resist problem
« on: August 21, 2017, 09:45:28 pm »
I used to generate  gerber files with Proteus 8.4 and never had a problem. Now I am trying Proteus 8.6 and noted some problems with the gerber files that it generates, at least with the solder resist mask. The pads of some components, in particular smd, are covered by the solder resist mask, al least when viewing with external 3d gerber viewer like http://mayhewlabs.com/3dpcb.
This also happens with some through hole component (for example SIL header connectors).

The same  happens with Proteus 8.5 so I assume that it is my fault.
Any idea of what can I be doing wrong?

Thanks
 

Offline electrolust

  • Supporter
  • ****
  • Posts: 380
  • Country: us
Re: Solder resist problem
« Reply #1 on: August 22, 2017, 04:14:22 am »
Check the guard gap setting for the pads in question.  "not present" = covered pad.

Somewhat painful to check, actually.

Place the footprint.  Decompose.  Select a pad to learn its name.  You might be able to edit the pad properties directly here, not sure.  If not, choose the appropriate pad type picker.  Choose the pad from the pick list.  Edit.
 

Offline pmaggi

  • Contributor
  • Posts: 19
  • Country: uy
Re: Solder resist problem
« Reply #2 on: August 22, 2017, 07:35:52 am »
That was my first thought. But it doesn't solve the problem. The first image (img1) corresponds to a gerber file made with version 8.4, the second one (img2) is the one that was done with version 8.6. Both with the same project.
If I inspect the gerber file with Proteus' gerber viewer everything seems to be ok, but if I use any other external program what I see is like the second image.
 

Offline pmaggi

  • Contributor
  • Posts: 19
  • Country: uy
Re: Solder resist problem
« Reply #3 on: August 22, 2017, 11:50:53 am »
This is the gerber file. Using Proteus' gerber viewer it seems to be ok, but with external 3d gerber viewers, the smd pads are covered by the solder mask (also some trough hole pads)
 

Offline spudboy488

  • Regular Contributor
  • *
  • Posts: 82
Re: Solder resist problem
« Reply #4 on: August 22, 2017, 09:37:13 pm »
Maybe it's your external viewer and how it does the rendering. I looked at the files with ViewMate and the resist layer looks fine. Red is the copper. Blue is the silkscreen. Green is the resist layer. The yellow is where the green and red overlap. You can see the green border around the pads where the resist is cut back a bit from the copper.
 

Online wraper

  • Supporter
  • ****
  • Posts: 7916
  • Country: lv
Re: Solder resist problem
« Reply #5 on: August 22, 2017, 10:01:30 pm »
Seems that you are using mayhewlabs gerber viewer. Although is seems like a nice 3D viewer in the first glance, it's a piece of crap frankly. There are so many incorrect display issues you can stumble on with it, it's not useful for checking for board issues.
Also which gerber format do you output? RS274X or gerber x2 which was added in 8.5 IIRC and may not be supported by gerber viewer.
 

Online wraper

  • Supporter
  • ****
  • Posts: 7916
  • Country: lv
Re: Solder resist problem
« Reply #6 on: August 22, 2017, 10:06:57 pm »
Just tried it on one of my boards already manufactured without any issues, also made by proteus 8.6 (gerber RS274X). Same piece of crap of incorrect display, on top of that most of the pads are just missing.
 

Online wraper

  • Supporter
  • ****
  • Posts: 7916
  • Country: lv
Re: Solder resist problem
« Reply #7 on: August 22, 2017, 10:56:37 pm »
BTW, your circuit looks like some sort of voltage regulator. Why tracks are so thin and there is no copper polygon for heat dissipation from vreg?
« Last Edit: August 22, 2017, 10:58:15 pm by wraper »
 

Offline pmaggi

  • Contributor
  • Posts: 19
  • Country: uy
Re: Solder resist problem
« Reply #8 on: August 23, 2017, 03:15:52 am »
wraper, thanks for testing it in your viewer and also confirming that a board that you already manufactured without any issues has the same problem with that particular viewer.
You are right, there is a voltage regulator (1117-3.3) in the circuit.
The board it isn't finished yet. I stopped it when I realized of the issue with the gerber file (fortunately just a false alarm). Anyway, the regulator works with less than 20% of it rated power, so it is fine without an additional disipation area.

The circuit is a lights smart switch, the big IC is an ESP32 module. I'm replacing the old ones installed in my house that I developed 5 years ago using PICs (16f1825) and nRF24 modules
The switches uses touch sensors, so that I'm using an ESP32 instead of ESP8266 in order to achive that functionality without using additional components.
 

Online wraper

  • Supporter
  • ****
  • Posts: 7916
  • Country: lv
Re: Solder resist problem
« Reply #9 on: August 23, 2017, 03:53:52 am »
Anyway, the regulator works with less than 20% of it rated power, so it is fine without an additional disipation area.
It's quiet a lot without any additional heat dissipation at all. There are different versions of 1117 but I would guess this is rated for for 0.8A current. BTW stating % of rated power and not actual power is counterproductive when that if without heatsink. Power can be tiny portion of max but already causing overheating. For LM1117 Junction-to-ambient thermal resistance 61.6oC. So if you dissipate say 200mW, that's already 12oC temperature rise. Dissipate 0.5w in a hot day and it's already running above 60oC. ESP 32 seem to consume up to 0.2A, if you are running from 5V, your vreg will be quiet hot.
« Last Edit: August 23, 2017, 03:58:28 am by wraper »
 

Offline pmaggi

  • Contributor
  • Posts: 19
  • Country: uy
Re: Solder resist problem
« Reply #10 on: August 23, 2017, 04:22:25 am »
Yes, you are right. ESP32 consumes about 120mA when connected to a wifi, and when it is transmiting it can reach up to 300 mA, but just in bursts. I have tested it and the regulator just get a bit warm, not too hot.
But I'll take your advice and provide some extra copper for more dissipation. Thanks
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf