Bottom B-Paste - no data, F.Paste missing some pads.. [updated]

I have generated all Gerberfiles as useally. But the file with ****-B.Paste.gbp is empty. Top paste is ok but no B-paste is shown. What do I wrong?

[EDIT by Joan]

Did you put SMD devices onto the Back of your board?
If the footprints of those devices are not from github, did you make sure they all have the paste layer activated in their pad settings?

1 Like

Are there any SMT parts on the bottom layer?

EDIT: Sorry, Joan beat me to it! As with all of these “what’s happening?! Why?” posts, it helps to have design files, namely your .kicad_pcb.

1 Like

Yes there are SMT parts on bottom. but no data in the B.Paste.gbp file.
Also pad settings are seems to be OK for all footprints.

Is there a way to create it?

Can you attach (or upload somewhere) the gbp file in question so we can have a look?

Did this work before?
What OS/KiCAD are you running?
Did you change anything between ‘when it was working’ and ‘it’s broken now’?

Can you get us a screenshot of one of the pad settings of a SMD that’s on the bottom layer?
Should look similar to this (taken with a footprint that sits on B.Cu):

Just by about 5 seconds… I’d seen mine uploaded and 5 secs later your’s got added below :blush:

Hi Everyone,

When i generated the Gerber files, B.paste layer is empty and F.paste layer doesn’t have all the components, I checked Pad settings and everything seems OK. I am not sure how to get these two layers correct. Is there a way to add there layers now some how? If not what can be the solution for components assembly.

Thank you everyone
BR, Shahid

I tried to upload but it said new users cannot upload attachments.

It didn’t work before, I didn’t know because before i was only ordering the PCB but this time they need it for assembly.

I am running KiCad 4.0.2 stable version.

I didn’t know if it was working before, so apparently did nothing, missed something since the beginning.

I went to Pad settings and found the problem. Now i can see the pad in .paste layer, BUT i have to do it for all the pads, Can i select somehow all togather and do it? One by one will take forever.

When i try to select multiple pads the option for pad settings disappears.

Thank you for the help and fast feedback.

BR, Shahid

Only outside of KiCAD in a text editor afaik.

A .kicad_pcb file on the inside looks like this for a 0805 resistor placed at the bottom layer of a pcb:

(module SMDx:C_0805 (layer B.Cu) (tedit 56AB8888) (tstamp 575F9AC4)
(at 22.31 15.962)
(path /575F9A8E)
(attr smd)
(fp_text reference C101 (at 1.15 0 270) (layer B.Fab)
(effects (font (size 0.6 0.6) (thickness 0.1)) (justify mirror))
(fp_text value C_100n-16V-X7R-kemet_0805 (at 0 0 270) (layer B.Fab)
(effects (font (size 0.6 0.5) (thickness 0.1)) (justify mirror))
(fp_text user %R (at -0.4 0 270) (layer Eco1.User)
(effects (font (size 0.3 0.3) (thickness 0.03)))
(fp_line (start -0.9 1.6) (end -0.9 -1.6) (layer B.CrtYd) (width 0.05))
(fp_line (start -0.9 -1.6) (end 0.9 -1.6) (layer B.CrtYd) (width 0.05))
(fp_line (start 0.9 -1.6) (end 0.9 1.6) (layer B.CrtYd) (width 0.05))
(fp_line (start 0.9 1.6) (end -0.9 1.6) (layer B.CrtYd) (width 0.05))
(fp_line (start 0.625 0.325) (end 0.625 -0.325) (layer B.SilkS) (width 0.15))
(fp_line (start -0.625 0.325) (end -0.625 -0.325) (layer B.SilkS) (width 0.15))
(fp_line (start -0.625 1) (end 0.625 1) (layer B.Fab) (width 0.05))
(fp_line (start 0.625 1) (end 0.625 -1) (layer B.Fab) (width 0.05))
(fp_line (start 0.625 -1) (end -0.625 -1) (layer B.Fab) (width 0.05))
(fp_line (start -0.625 -1) (end -0.625 1) (layer B.Fab) (width 0.05))
(pad 1 smd rect (at 0 0.95) (size 1.4 0.95) (layers B.Cu B.Paste B.Mask)
(net 1 VCC))
(pad 2 smd rect (at 0 -0.95) (size 1.4 0.95) (layers B.Cu B.Paste B.Mask)
(net 2 GND))
(model SMDx/C_0805_H1-35.wrl
(at (xyz 0 0 0))
(scale (xyz 1 1 1))
(rotate (xyz 0 0 0))

I marked out the important bits.
Let the editor (notepad++ is good for this) search for (layers B.Cu B.Mask)
I assumed there that this string of text is missing B.Paste in your case
After that’s found, replace that phrase with (layers B.Cu B.Paste B.Mask)
Make a copy of the kicad_pcb file before you do this!
Then reload the file and cross your fingers :wink:

Joan_Sparky, That worked apparently, In case if i came up with any problem later i will post it here.

But thank you so much, You are the man!!


Interesting, I just noticed the same thing, lots of SMD components on the bottom yet kicad doesn’t even offer me the B-Paste layer, only mask, copper and silk screen!

Looking further into it, my standard footprints like 1206 resistors have the F-Paste layer checkbox ticked, however, in my last few projects, none of the B-Paste info is there, as if if that flag got deleted when I checked the box to place the component on the back.

Just tried to do the same thing again with a test board and now the flag is still there, even after switching the item to the bottom. Very odd, indeed.

Where is the bottom paste layer missing? You do not give any information that we can use to help you. (Kicad version, in which output format or program is the bottom paste layer missing? How do you know it is missing?)

Now i try to help you even without info. Be aware that i make a lot of assumptions here. (I assume there is just a misunderstanding and you never looked at the gerber outputs)

Footprints are typically designed as if they are placed on the top side of the pcb.
This makes it easier to design them as you then to not need to mirror the measurements.

To get them to the bottom side you use the flip function within pcb_new. (I think you did this as you mention switching to the bottom)
This takes care of moving all F.xxxx layer info to the B.xxxx layers and mirrors the part for you. (Mirroring is necessary because you look through the pcb from the top. Write something on a glass pane and try to read it from the back side afterwards.)

You should also notice that the colors of the pads change from the color given to the top side layers to the colors of the bottom side.
If you have no paste clearance and the focus is on anything other than the paste layers you will not see paste in pcb new. Click on the layer name in the right toolbar to give it focus. (Put one footprint on top and flip one to the bottom. set the focus on b.paste and f.paste. You should notice a difference. But only if the layer colors for these two layers are different. They are by default but you might have changed it.)

If you flip the part to the bottom the paste properties dialog still shows you the pad as if it is on the top side.
In kicad nightly there now is a very visible warning above the layer selection dialog to make this more clear. It reads: “Parent footprint on board is flipped. Layers will be reversed”

Thanks a lot for quick help, Rene.

I’ve been using kicad fro a few years now and that might be pat of the problem:

I’ve had two layouts that I kept updating and they were not set up correctly: the B.Paste layer was turned off in the Layer Setup. On my newer projects it was turned on and flipping components to the bottom retained that flag.

I’ve sinced corrected the .kicad_pcb files and send it back to the manufacturer.

Thanks again for your time and explanation, I’m sure it’ll come in handy for someone at some time!

1 Like