How to make this shape ?
Center pad: place normal pad and set rotate to 45deg.
Corner pads: combine with 3 crosssected pads.
3 Likes
You wonât get the sharp edge for pin 1 done in pcbnewâŚ
1 Like
Thank you ! Iâm doing that , but when trapezoid delta is set to equal to the size of the pad it report error " the trapezoid is set too large"
ĺ¨2016ĺš´05ć09ćĽ 03:17ďźKerusey Karyu ĺé:
|
| | keruseykaryu
May 8 |
|
|
Center pad: place normal pad and set rotate to 45deg.
Corner pads: combine with 3 crosssected pads.
|
Visit Topic or reply to this email to respond
To stop receiving notifications for this particular topic, click here. To unsubscribe from these emails, change your user preferences
Iâm trying to create that footprint
I can created this part of the pad
But How can I determine its placement origin position, or how can I move the origin of the pad ?
1 Like
Man, what a bitch (the smallest step in mm grid is too big already for this, the imperial grid goes smaller, but is not really useful as the values in mm donât come straight).
Enjoy:
PX2SON.kicad_mod (2.3 KB)
And in case anyone wonders how I got those dimensions right, here you go (in case you want to do this yourself):
1 Like
But you could try to do it with FreeCAD as well (and Iâd probably have, but Iâm used to that tool and got access to it, so I never have the need really to need to learn FreeCAD).
PS: thanks for the trapezoid idea for the triangle⌠thatâs why I made the footprint then eventually.
PPS:
I tried placing them manually as good as possible and the last tiny bitâs of movements I then did via the coordinate input for the pads via trial&error, until they did fit on the highest zoom level that is possible in the editor.
Anything below that resolution wonât matter for normal fab houses anyway as their tolerances and accuracy will be worse than that.
I was told long ago, that sharp points like the original pin 1 pad, were discouraged in PCBs as they caused etching problems.
More recently I would worry about them triggering the dreaded lead free solder tin whiskers, causing a short
I donât know why but the layout example in the first post is form tlv713p, the final footprint is from tlv733p
@davidsrsb
I think sharp edges up to 45 deg are ok, anything sharper than that and you can have problems because it getâs too thin then for the reasons you listed.
@sprhawk
You will get DRC errors and have trouble connecting tracks to those pads.
Set the pin/pad number for all pads that are supposed to be âoneâ (as you can see in my example up there).
Also, unless you have a very good reason to do it, you might want to abstain from setting the solder mask margin in the footprint⌠it usually is done globally per pcb layout (otherwise you might include footprints into your layout that the fab cant make as you donât easily âseeâ what kind of margin the footprint brings.
Oh and you should add some device outline on F.Fab and a total placement outline (safety margin) for the overall footprint on F.Courtyard.
1 Like
Thanks for your correction.
I donât understand for the solder mask: whatâs your mean to define solder mask globally ?
and what is F.Fab and F.Courtyard ?
I see, you mean set the mask clearance with 0 to use a global settings values, right ?
F.Fab is for the manufacturing
F.Courtyard for Testing, but how to use with Courtyard ?
Yes, mask clearance to 0 for the footprint to use global settings when you go to fabricate the board⌠every boardhouse has got different abilities what they can do for smallest clearance and accuracy (also depending on cost), this way you can adapt the whole pcb in one go to the particular board house if you set this to 0 in the footprint (some footprints need special settings, but this should be the exception, not the rule afaik).
x.Fab is for you to see the real average outline of the device in question (some people even draw the pins on there like @Andy_P) . It might also be used for documentation purposes when you need some overview plan for the board and what sits where and how big it is (when you print out a population diagram for hand soldering for example).
x.CrtYd is for you and depicts the outer dimension of the footprint AND the device PLUS some margin (there is a footprint design guide for KiCAD on the website somewhere in case you want to know more, @keruseykaryu should have a link handy), so that when you place the component in a layout you donât go below that threshold (unless you know what youâre doing) so it can be assembled by a pick&place machine (or someone with a vacuum pen ;-)).
Some people use x.SilkS for that as well or instead, but x.CrtYd is there for that purpose alone and usually doesnât make it into the gerbers.
1 Like
@keruseykaryu can you find the Kicad design guide as @Joan_Sparky mentioned earlier ? I didnât find it.
If @Joan_Sparky had in mind my simple tutorial it will be useless to you because it was written in Polish. 
And currently it has 6 years old.