A very nice feature “created pad from selected shapes” was removed from V7?
Under Create from Selection is available only the option Arrary… any hint?
Here is a comparison between V5 and V7
A very nice feature “created pad from selected shapes” was removed from V7?
Yes. The developers are very mean and wanted to annoy all footprint-designers who need custom pad shapes.
Fortunately they added another feature which is equally helpful:
- click & select the central normal pad which should serve as the anchor for your custom pad shape
- RMB-click → context menu–>Edit pad as graphic shape
- footprint-editor canvas changes into “pad edit mode” (see yellow warning bar at top of screen)
- now move all custom copper-items onto the central pad. All copper-items which connect to that pad form later the custom pad shape.
- It’s enough if a copper-item connects to the anchot pad through another copper-item, a direct connection to the pad is not necessary
- you can use any copper-shape (line, circle, arc, rectangle, polygone unfilled or filled)
- If you are finished with your custom form: RMB-click–>context-menu–> Finish pad edit mode
I first tried to link to the kicad v7-documentation, but the “custom pad shapes” section is empty. Maybe these sentences can be used as start.
3 Likes
Yes this is frustrating indeed… but thanks for your post I discovered a shortcut: if the pad and the copper area already overlap, by selecting the pad then enable edit and then disable edit, the custom pad will be created (obfuscated but doable).
Developers, please bring the feature back; it’s nice to have such option in the context menu…
Thanks,
Andrei
Yes this is frustrating indeed
I thought my sentence was exaggerated enough to be recogniced as joke. For me the new version works well.
Developers, please bring the feature back; it’s nice to have such option in the context menu
I think the new behaviour is not so much different than the old. New name, but still in the context menu. Maybe you need only to spend some time to get familiar with the new context menu entry?
If you really want the old behaviour back you have to open a gitlab issue. But I think you will need more arguments than “I liked the old implementation much more” to convince the developers.
As I say… frustrating; I have this part (see bellow); the pad is composed by a trough hole and an SMT pad on the top layer. When I do Edit pad open/ close it creates a new pad and replicate the top shape on the bottom layer as well which I don’t wish.
In contrast, by editing the footprint in V5 I was able to create a pad3 that has a trough hole and a SMT different surface only on the front layer (I place a circular small SMD pad on the front then combine the 2 surfaces to create a new pad)
It can be done (probably) in V7 but with headaches: first you need to move the thought hole to avoid overlapping then to create the new SMT pad then move-it back; create pad from selected shapes was a very nice/ quick feature…
I also found the “Create pad from selected Shapes” easier to work with. Especially when you already have some graphics on the PCB, and want to add that to a pad.
I also discovered by accident that just entering and exiting the “Pad Edit Mode” changes what graphics are part of a pad, depending on whether that graphics overlaps the pad, which is a workable hack or accident or maybe even by design.
But this changed feature is also relatively new in KiCad, and I expect it to improve over time. For example, having a function to first enter pad mode, then select some exisiting graphics and add that to the pad may be useful. But I have not thought about this enough to make a decent proposal for this on gitlab.
1 Like
Yes enter select one element and then exit to pad edit mode had the consequence of combining overlapping pad that might be not wished; anyway I understand that now it’s different but we have to consider if that is an improvement or a drawback; I’ve got no clue of the reason of change… maybe it’s a good one.
just entering and exiting the “Pad Edit Mode” changes what graphics are part of a pad, depending on whether that graphics overlaps the pad, which is a workable hack or accident or maybe even by design.
Reading between the lines of programmer-answers on gitlab discussion I think it’s by design. The “Pad Edit Mode” just combines all copper-elements which overlap & have a connection to the central anchor pad.
For example, having a function to first enter pad mode, then select some exisiting graphics and add that to the pad may be useful.
That would be more similar to the old behaviour (I think, I only changed to kicad with v6 so never used the old function).
But thinking about the custom pad I find the current decision to simply take all copper which is connected to the central pad as part of the “custom pad” very reasonable:
- if copper connected to the pad remains as “not part” of the pad this will always create short circuits - so this case should not happen at all for normal footprints
- if copper unconnected to the pad is selected to be a part of the pad this will always create unconnected problems - so this case should not happen at all for normal footprints
So the decision “take all connected copper as the custom pad” is understandable.
I admit that the name “Pad edit mode” (*1) is not the best, the function to create such custom pads for the first time is not self-explanatory. But for a complex software I don’t expect to have all functions suitable for beginners. (for instance to explore “custom pad mode” in eagle and Altium circuitstudio I also needed to consult the help function).
*1: “pad edit mode to create custom pad shapes” is lightly to long for a context menu entry…
One more thing: if you are not in pad edit mode, you have a context menu “Create from Selection…” Shouldn’t be better if on that menu to have a submenu called create a custom pad?
As it is today, works but obfuscated… I’m not sure what to lead to this design changing decision but I assume is a strong one. So we cannot have a strong good case beside frustration of asking to change-it, but if the developer see the post maybe will re-think.
Personally beside others valuable things I’m very glad that the 3D viewer in 7 is much faster for MAC ARM (as is native now) with is awesome! KiCAD is now on the direct path to compete head-to-head with the big guys in this field and the functionality become neat and sleek (beside that is free).
At first thought this seems a logical Idea and I like it, It does have limitations, and complications.
I agree with that, and with:
There seems to be no help files for either the Symbol editor or the Footprint editor:
paul@cezanne:/usr/share/doc/kicad/help/en$ ls -hl
total 1,5M
-rw-r--r-- 1 root root 509K Mar 11 18:03 eeschema.html
-rw-r--r-- 1 root root 46K Mar 11 18:03 gerbview.html
-rw-r--r-- 1 root root 114K Mar 11 18:03 getting_started_in_kicad.html
drwxr-xr-x 4 root root 84K Mar 11 23:19 images
-rw-r--r-- 1 root root 52K Mar 11 18:03 introduction.html
-rw-r--r-- 1 root root 93K Mar 11 18:03 kicad.html
-rw-r--r-- 1 root root 42K Mar 11 18:03 pcb_calculator.html
-rw-r--r-- 1 root root 451K Mar 11 18:03 pcbnew.html
-rw-r--r-- 1 root root 69K Mar 11 18:03 pl_editor.html
And they are also not listed on:
Apparently these editors fit so well in the KiCad GUI / Workflow that I have never even tried to read documentation for them 
Link: https://docs.kicad.org/7.0/en/pcbnew/pcbnew.html#creating-and-editing-footprints
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.