Front Silk Screen incorrect in Gerber File

The Front Silk Screen in the PCB editor is not the same as that renders in the gerber file.

I cannot post the 2nd image as I’m a new user and I’m limited to 1 image

I’m using Kicad 4.0.6 on windows 8 64 bit

The second image:

Looks the same to me.

In KiCad, PcbNew, turn off all the layers except for the Front Silk Screen layer and you will see only that layer.

KiCad provides other layers, to use for layout, such as CourtYard and Fab. These are not normally needed by the PCB manufacture to create the physical boards.

1 Like

Take a look in the R18 and R19 location, you will see what I mean.

A big clue is the color of your screen shots.

I’m fairly certain that the light blue color graphics are the Silkscreen; and the yellow graphics are another layer (possibly the Fab layer).

Turn every layer OFF, except for the Silkscreen layer.

Also under the “Visibles” panel, select the “Render” tab and de-select “Pads Front”,“Pads Back”, and “Anchors”.

Some of the “render” selections are a bit un-intuitive.


Yes, try to show a screen shot of ONLY the silkscreen layer. Even if the color assignment table is visible it is often difficult to tell what is on a single layer.

It also looks like your Gerber plot has at least two layers mixed together. The repeated notations such as “D5”, etc, look like tool codes for the various hole sizes.

Did all of your footprints come from the standard KiCAD libraries? About a year and a half ago I noticed that some of the standard KiCAD footprints had problems with the silkscreen but I thought that had been corrected.


1 Like

I actually saw that, but did not want to in any way further confuse the issue.

The instructions that I provided for KiCad to show only the the proper items on the Silkscreen layer should be what is expected to be on Silkscreen layer of the Gerbers.

Should having to turn off all the extra visibles be filed as a bug report?

1 Like

Those are the aperture ‘D’ codes. In GerbView select the “Render” tab and deselect “D Codes”.


Thanks, you have clarified why the Silk Screen is different from what I expected. I did not have “references” selected for render. So I was moving

However, it has raised a further issue. If I have Front Silk Screen selected as visible, why do I need to modify the “render” selection to see all of the Front Silk Screen?

As Sprig indicated [quote=“Sprig, post:5, topic:6569”]
Some of the “render” selections are a bit un-intuitive.

I think “a bit un-intuitive” is a “bit” understated. With ALL renders off and ALL layers ON this is what is displayed:

While not a bug, I think it’s a feature that needs to be reconsidered.

It’s an odd world… :slight_smile:

That’s what I get when everything is turned off. I’m on Win10, May12th nightly, OpenGL canvas.

Yeppers, I’ve done that too, and wondered why if all the LAYERS were turned off … why is anything being displayed?

I suspect this is not an easy fix for some oddball reason.

I use the render tap mainly to hide references and values while I layout the pcb. This way I have less stuff that distracts from working on traces.

My footprints are a bit different though. I have the main reference on the fab layer and the secondary on silk. I hide the silk layer while I work on the pcb. (I use the fab and courtyard layer to tell me where which component is.)

This workflow is inspired by one @Joan_Sparky described a long time ago. (I can’t find the post now.)

1 Like

Can live with the status quo. If there only was an easily accessible save/recall mechanism for layer visibility settings (sigh).

1 Like

I personally don’t have VAL** or REF** on silkscreen, for me those are on the F.Fab layer and even then I switch them OFF in the render tab as the only time I need them is for doing a documentation of the board.
The KiCAD libs have those fields on the F.Silk layer as most people want them visible on the board.

For actually doing the layout one needs them sometimes, that’s why I have another smaller REF** field (text field with %R) on the Eco1.User layer - which is free to use for anything.
By using an extra layer with it’s own bright color those values stand out and are easily depictable.
I keep their size at h0.6,w0.5,t:0.06 so they fit into 0604 outlines and don’t distract during layout.
The official KiCAD libs have something similar on the F.Fab layer.


  • REF**, VAL** can only occur ONCE per footprint and adhere to the render tab switches for References/Values as well as to the visibility switch of their respective layer.
  • %R, %V can appear several times per footprint and will ONLY adhere to the layers visibility switch and not to the render tab switch for References/Values.
1 Like

On a slightly related note, I have just taken delivery of the first 3 boards I designed with Kicad. Very happy with the result but somehow I managed to un-tick “plot footprint references” on one of the three resulting in the footprint reference text missing from the silk screen on that board. Not a disaster but shows you do have to pay attention to detail.

It is probably relatively easy to turn visibility on /off in a python script.
(Once youve figured the syntax out)
In one of the threads I read it’s also possible to add menu buttons to KiCad with Python.

A relatively easy way to do this is probably to stude the footprint wizards

LayerVisibilitySet script is on its way! Should release in the next few days. There are bugs in the nightly that will make it less useful for the moment, but I assume (hope?) those will be fixed eventually.

1 Like

Which is why viewing the Gerber plots with GerbView or equivalent should always be part of your process


Agreed, but even then you need to pay attention because other text notations you may have added can still be seen. So if your coffee level is depleting you might assume that all text is on because you can see some text.

Depends on whether you are really serious about using that last-look as a true QA task, or just dismiss it as another box to check before you send the files off to the fabricator.

My fear at that stage of the process is that some reference designator has been parked on top of a solder pad, so I’m certain a total absence of reference designators would be noticed.