Thermal Relief Generation Issue

[Don011]

I recently updated to 5.1.0 and I’m really impressed with all of the improvements that have been made. However, I have just noticed an interesting issue with the generation of thermal reliefs when creating a ground pour. I have a large muti-way through hole connector and a ground pour around it that connects to various pins. This board was last edited using KiCad 5.0.0 and the thermal reliefs between the pour and the ground pins look as you would expect, all four spokes are present where possible.

After opening the board in KiCad 5.1.0 and updating the zone fills some of the thermal relief spokes are no longer being generated properly. They have a weird “double bump” shape and do not actually connect.

I have tried messing with the zone clearance settings but I can’t seem to get the thermal reliefs to be created properly. The zone clearance settings are:

There are no custom clearance settings for the footprint.
Is this a bug or am I doing something wrong? Any help would be appreciated.

[Sprig]

@Don011

Is this a bug or am I doing something wrong?

Those settings are very large, perhaps double what they should be. Check by setting them all to 0.1mm and see what results you get.

Note however, that these need to be set to what your Fab House can actually create.

[PCB_Wiz]

@Don011

After opening the board in KiCad 5.1.0 and updating the zone fills some of the thermal relief spokes are no longer being generated properly. They have a weird “double bump” shape and do not actually connect.

Hmm. the strange thing here is the some.
Are those all from the same zone outline ? Are all pads the same ? Any pads have routed tracks ?

Pins 13 & 17 look ok, but 9 & 10 have X-axis issues ? - so spot-the-difference should give a clue.

[Joan_Sparky]

Can you check the local pad clearances for #10 and #13 for example?

[Sprig]

@PCB_Wiz

Hmm. the strange thing here is the some.

Well, that depends.

Some versions of KiCad used the same orientation for the Thermal Relief copper connection.

However, some versions of Kicad alternate the copper pour by 45 degrees to further thermal relief any adjacent pad.

[Rene_Poschl]

There was a bug in 5.1.0 that meant thermals for oval pads where not correctly made. Check if the effected pads are oval or circular. If this is the case try updating to 5.1.2 or change the pads to circular.

[Sprig]

The OP posted a file that looked like through hole circular pads.

I’ve had no issues with Windoze 5.1.0 and a recent test build with rounded rectangle pads and thermal reliefs.

[Rene_Poschl]

oval pads with x and y direction the same size lool like circular but are seen by DRC as something different. (By the way am i blind or did he post the file in private to you as i can not see one here. The only thing i see is two screenshots.)

[Sprig]

@Rene_Poschl

The only thing i see is two screenshots.)

There are three(3) screengrabs.

The third shows the settings information. The OP settings broke one of my projects in the same way.

[Rene_Poschl]

@Sprig

There are three(3) screengrabs.

The third shows the settings information. The OP settings broke one of my projects in the same way.

I see i need my coffee. (I somehow forgot about that one. Sadly it does not include the information needed to see if the pads are circular or oval as that setting is at the very top of that dialog and possibly even on a different tab.)

[Don011]

There was a bug in 5.1.0 that meant thermals for oval pads where not correctly made. Check if the effected pads are oval or circular. If this is the case try updating to 5.1.2 or change the pads to circular.

This seems to be what happened. The pads on that connector were oval shaped but had the same X & Y size to make them circular. Changing them to circular and updating the zones fixed the problem. The thermal reliefs have also changed from + shaped (oval) to x shaped (circular).

Is the circular option new? This footprint was made by someone else in 5.0.0 and some of the through hole pin header footprints in the default library also use oval instead of circular. I would have though that the circular option would have been used if available.

Also I did try the other suggestions but didn’t find anything. I saw this while in the middle of replying.

Thanks all for the help.

[Rene_Poschl]

@Don011

Is the circular option new?

No always was there. If the footprint is from the official lib then it might have been scripted before i added a check to the pad class to ensure that such pads are circular if the x and y direction is equal