Have only the PCB 5 or (FR4) on the board

Hi everyone,

I’m trying to make some PCB art. I have a couple of drawing and have more or less figured out how to have the layer on the silk, mask, copper, edge cuts, etc.

If I want nothing on the board (no copper, silk, mask), I need to use keep out and draw maybe a square, a circle, triangle and more.

But my question is the following, I want to put a car that I have draw on the board being on the PCB (No copper, silk or mask). Knowing that the car is already draw (by me), How should I proceed?

Thank you for your help and time with this.


Another way is to directly import .dxf files into KiCad.
.dxf files can be exported by most CAD packages.
Unfortunately there seems to be a bug in the current Stable KiCad V5.1.5 for .dxf import. If KiCad can not read the file, and complains it’s “empty”, then apparently you have to “explode” the drawing, and import it as separat lines and arc segments.
There has been a post about this in the last few days, so search this forum for more.

1 Like

thanks for your uick answer paulvdh

I should use SVG2shenzen? I have tried to use this plugin but have some errors. When clicking on prepare document, I have the error “File “prepare.py”, line 5, in
import inkex”. I think that’s a python library. I thought I installed the plugin package correctly but having this error. Any ideas anyone on the subject?

About the dxf method, after importing them into kicad, what layer should I place it into so there is a no copper, no silk, no mask where the image is?

I will check for the previous posts you are talking about as well.

Let me know if you have any other tips.

Thanks for everything.

I don’t understand what you really wont.
It looks that you have your draw already done at the board and you need PCB only to fix (glue) that board to that PCB.
I suppose it should be possible to order empty PCB by giving the PCB factory only its dimensions. Probably not by using any automatic ordering system which will ask for gerbers but by mail they should be able to just do the empty PCB with X*Y dimensions.
But using KiCad you should only draw a rectangle at Edge.Cuts layer specifying the PCB dimensions. And then Plot that layer to Gerber.

Hi Piotr,

Thanks for your answer.

Let me try to explain. I know it’s hard to explain and understand behind a screen.
I have a drawing I have made on Inskcape and want to do PCB Art with it on my board.
You know put the drawing on the silk screen ( e.g: a logo), or on the mask, the copper or the PCB ( FR4). Each layer being on one another (silk, mask, copper and the PCB), you may need to remove the mask if you want to draw on the copper (so people can se it), or remove the mask and the copper if you want to draw on the pcb.

How do I remove the mask and the silk to draw on the pcb with the drawing I have made. here isa example I have found on the internet. that may maybe help you understand a bit better.

PCB art

You can see her skin is brown (it’s the pcb), then you have copper sometimes in the hair. But for the skin, they remove the mask and the copper.
My question is the following: How do we remove the copper and the mask like a keep out zone but with a drawing ?

I don’t think you have the concept of what you want squared with the way PCBs are manufactured. Try thinking of it this way:

  • Everywhere you want the bare PCB showing, remove copper (i.e. fill copper everywhere except where you want the bare PCB showing.
  • Everywhere you want bare PCB and copper showing, fill in the mask color (solder mask is the only negative layer).
  • Everywhere you want silkscreen, fill in the silkscreen.

With those techniques in mind, run your image “color separation” masks through the Bitmap to Component converter. (Or if you want to skip the potentially lossy conversion from Inkscape to bitmap back to KiCad vector, you may want to use something like SVG2shenzen.) You may need to save the copper layer to something like “Eco1” and then hand-modify the resulting file to move all the graphics to the F.Cu layer. Load the three resultant components into PCBNew and line them up. Check the 3D viewer to see if it looks like what you want (both soldermask and silkscreen colors are customizable in the 3D viewer).

When having the board made, pay attention to the copper finish type. ENiG will get you a gold finish on your copper, HASL will get you a silver (solder) finish on your copper, or you may be able to request no copper finish to have bare copper. You can also tell your board house not to bother with an electrical test… (Depending on the board house, skipping the electrical test may save you some money.)

EDIT: Note, I have not attempted this myself. Take my above advise as a starting point. There may be some subtle details that I haven’t covered because I’m not aware they exist. But, hopefully this can get you started in the right direction.


@SembazuruCDE gave you the necessary information, but it may help to rephrase the same with other words.

This is the order of manufacturing:

  • FR4 is on the bottom.
  • Copper is on top of that.
  • Mask is on top of that. See How does solder mask layer work?. “Solder mask” is really physical substance and the mask layer in the software is negative of physical mask.
  • Silkscreen is on top of everything.

As of the visibility and looks:

  • Copper is fully opaque.
  • Mask is semi-transparent, so copper under mask may look different than no copper under mask.
  • Depending on the manufacturer, there are color choices for mask. Some manufacturers can even use several colors for one board.
  • Silk is practically fully opaque.
  • Depending on the manufacturer, there may be color choices for silk.
  • There are finish choices for copper.

If you want the bare board to be visible, the layers in the software are:

  • No graphics in F.Cu (copper) or F.Silk
  • Graphics in F.Mask

I think the most difficult part is getting the mask layer right. If you want to draw with thin stripes of mask substance on copper and/or bare board, you have to have large areas of graphics in the software Mask layer and thin stripes of no graphics. For copper and silk it’s just moving your original graphics to the layer graphics.

Do you have your original design in SVG format and can you share it here?

1 Like

The cool thing about KiCAD is that you can always check the effects of what you are doing with the 3D Viewer and even select the color of the individual elements (Silkscreen, Base Material, Solder Mask, etc.)

Doing a quick test I go the following:

So, if you want to show a car with the color of the FR4, you have to not have Copper (F.Cu), not have Silkscreen (F.Silk) and to draw the form of your car in the solder mask (F.Mask), that way the mask will not be placed there, showing the raw material below (upper row, “Mask” square).

Probably you have seen this links, but the process is better explained here:

1 Like

I still don’t understand your question.
For a promotion of our one device (RFID reader with painted glass front) I have done once the PCB with some gold (gold plated copper) text information (and written along the circle) to be used instead of standard PCB with terminal blocks. So I understand that you can get several colors at PCB, but in your first post there are two times you wrote:

So I understood - you wont to get a clear PCB without anything on it - no copper, silk or mask means for me: only the basic laminate. Such PCB is one colour. So as you wont such pcb what for you can need it in context of art. But what you need you already draw on the board so may be you just wont to fix this board to PCB.

Now I still don’t understand. May be:

  • you wont the PCB factory to do for you that PCB with your picture (but to this point the text of No copper, silk or mask does not fit),
  • you wont the PCB full covered with copper mask and silk to do your picture (based on already drown at your board) by manually removing selected layers (to this point the text of No copper, silk or mask also does not fix perfectly but may be you had in mind - no pattern already done at copper, silk or mask.
1 Like

You guys are rocking. Coun=ldn’t be better explained. :sunglasses:
Thank you all so much for your explanations and patience

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.