ALTIUM mounting holes question

Go To Last Post
18 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi there,

I am an ALTIUM PCB designer user. For years now, in order to place a mounting hole (let's say a screw hole) I use to place a multi-layer pad and set it's SHAPE SIZE = HOLE SIZE. The final PCB result is just a hole (without coper).

I set the Minimum Annular Ring rule to 0.125mm. So when I make a Design Rule Check, ALTIUM prompts me a violation like : " Minimum Annular Ring: PAD HOLE1 (X mm, Y mm)Multi-Layer (Bottom Layer Minimum Annular Ring=0mm "

This is a problem for me, because the last weeks, my PCB manufacturer added a new rule to his GERBER check program and tells me that my PCB has some problems with the holes because of the Minimum Annular Ring rule.

I would just like to ask if there is any other way to place a HOLE in Altium, except adding a PAD. ???

Thank you.

Michael.

User of:
IAR Embedded Workbench C/C++ Compiler
Altium Designer

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Michael,

you can also place a non plated hole if it does not have to be attached to the copper.
place the hole and then when you double click to set the parameters, like hole size, there is a check box 'plated'
if you uncheck that and make the copper (top richt part) same or less then the hole size itself you get a non plated hole.....

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hahahahahahaahaaaaa........OMG,

Thank you very very much. I realy never show that option !!!

God bless you.

Michael.

User of:
IAR Embedded Workbench C/C++ Compiler
Altium Designer

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

upppsssss.....

I did this, but the Design Rule Check prompts me the same Violation.

I am going to send the new GERBER to the manufacturer hoping for positive news this time.

Michael.

User of:
IAR Embedded Workbench C/C++ Compiler
Altium Designer

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

strange,

just placed a pad on the PCB I have.
Set hole size to 30mil and size and shape to also 30mil.
Made the net to no net. Set non plated and repoured the planes. run DRC and get 0 errors.

You do not accidentally have another pad on the same location that still is plated?
non plated holes should never give a minimum annular ring error as there should be no copper in there at all.....

btw did it on AD13.2.. but as far as I know AD9 & 10 work the same

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I always set my pad size to 1 mil x 1 mil and I've never had an annular ring DRC error. Maybe give that a try?

Jeff Nichols

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Not Altium, but in the package I use (easyPC) I set my shape size to be much smaller than my hole size. So for an M3 mounting hole I have a 60mil pad with a 122 mil drill and set it to un-plated. I get a warning when I design the PCB symbol for the part but never on DRC or from my PCB manufacturers.

#1 Hardware Problem? https://www.avrfreaks.net/forum/...

#2 Hardware Problem? Read AVR042.

#3 All grounds are not created equal

#4 Have you proved your chip is running at xxMHz?

#5 "If you think you need floating point to solve the problem then you don't understand the problem. If you really do need floating point then you have a problem you do not understand."

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

can't you just tell the supplier to ignore those errors, as you are aware of them and they are intended in your design?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

midea31 wrote:
can't you just tell the supplier to ignore those errors, as you are aware of them and they are intended in your design?

That is not so easy, you are violating design rules from the PCB manufacturer. If something turns out to be wrong in the end who is responsible for the useless PCB's you or the factory?
You can ignore errors in your own design as then you are responsible, but if the manufaturer says there is an error most of the times you need to change.....

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If he has been doing this for a long time and making PCBs well and good with his method, then how does the supplier adding a new checkpoint make his designs any less reliable?

(of course I have only ordered pcb fabs twice and only tens in quantity, so i am hoping to learn from this)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi guys,

The problem is solved following meslomp's suggestion.

Quote:
you can also place a non plated hole if it does not have to be attached to the copper.
place the hole and then when you double click to set the parameters, like hole size, there is a check box 'plated'
if you uncheck that and make the copper (top richt part) same or less then the hole size itself you get a non plated hole.....

ALTIUM still gives me the violatioin: Minimum Annular Ring, but the PCB Manufacturer has no problems anymore.

Thank you all.

Michael.

User of:
IAR Embedded Workbench C/C++ Compiler
Altium Designer

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Michael,
glad the factory problem is solved.

it is strange that you get an annular ring error on a non plated hole...
Perhaps take some time to investigate what is going on.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Sounds like a nice administrative public service solution.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I wonder if the gerber or NC drill output (which is used by board manufacturers) allows for the same error detection. Probably not. The gerber wouldn't contain any of the PCB file design rules so presumably the manufacturer would apply their own manufacturing rules to validate if they can actually make the board.

Steve

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

the board manufacturer checks the generated gerber files.
Part of those files is a drill table. This table tells whether a hole is plated or non-plated. The gerber check tools keep that in mind when doing the gerber check. So they do not see the design rules given into your design.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Gerber cam software can do a huge variety of artwork checks covering issues such as acid traps, component legend over pads, solder mask expansion, minimum distances between adjacent features belonging to same net and or differing nets, etc.. to ensure maximum yield in production.
The part of board designers work which may not be addressed by PCB CAD software.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You can use plated holes for screws. Make the pad bigger than the hole so that the Minimum Annular Ring rule will no be violated.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

This cannot take place for my case for electrical reasons.

Michael.

User of:
IAR Embedded Workbench C/C++ Compiler
Altium Designer