Maker Pro
Maker Pro

Orcad: carbon pad

E

engcif

Jan 1, 1970
0
Hi,

We are working on a telephone circuit layout. We have drawn a carbon
pad for silicone keypads in layout and attached the drawing to a pin
so that the whole drawing became a pin that can be used as a
footprint. But we are not so happy with our carbon pad footprint. Is
there a better/common way of doing this or any tricks?

Thanks everyone.

Engin
 
Q

qrk

Jan 1, 1970
0
Hi,

We are working on a telephone circuit layout. We have drawn a carbon
pad for silicone keypads in layout and attached the drawing to a pin
so that the whole drawing became a pin that can be used as a
footprint. But we are not so happy with our carbon pad footprint. Is
there a better/common way of doing this or any tricks?

Thanks everyone.

Engin

If your switch pad is moderately complicated, create the pad outlines
in a 2D drawing program like AutoCad or the drawing package that comes
with layout. You can import the the graphics into Layout via a DXF
import. You need to look at the maxdxf.ini file in the Layout
installation directory for instructions for layer names. When you
import the DXF into a Layout footprint, you will have obstacles. Edit
the obstacles to place them on the proper layer, give them the proper
obstacle type, and attach it to a pin. You will have a beautiful
footprint which will draw oohs and aahs.
 
M

Marra

Jan 1, 1970
0
If your switch pad is moderately complicated, create the pad outlines
in a 2D drawing program like AutoCad or the drawing package that comes
with layout. You can import the the graphics into Layout via a DXF
import. You need to look at the maxdxf.ini file in the Layout
installation directory for instructions for layer names. When you
import the DXF into a Layout footprint, you will have obstacles. Edit
the obstacles to place them on the proper layer, give them the proper
obstacle type, and attach it to a pin. You will have a beautiful
footprint which will draw oohs and aahs.

Not convinced this will work as the final pad has to be able to be
described by the Gerber command set.
Just tweak the pad until it is right in orcad.

www.ckp-railways.talktalk.net/pcbcad21.htm
 
J

Joel Kolstad

Jan 1, 1970
0
Marra said:
Not convinced this will work as the final pad has to be able to be
described by the Gerber command set.

That's just a question of the right conversion programs. Starting with
something like DXF, you can have something like CorelDraw output HPGL (it'll
convert all the fancy curves, fills, etc. into the simple "strokes" that HPGL
supports), and from there something like GerbView can convert HPGL to Gerber.
Most PCB packages can import Gerber.

Of course, many PCB packages can import DXF as well, although which commands
they support is often limited. Pulsonix, for instance, doesn't support the
DXF "SPLINE" command, so I use the approach described above.

You know the use of ALL CAPS on drawings/PCBs have been slowly dying ever
since the point where Xeroxing drawings (one of the main reasons ALL CAPS were
used historically) became uncommon? :)

The way you label nets is similar to how the LabView guys like to do it...

---Joel
 
Q

qrk

Jan 1, 1970
0
Not convinced this will work as the final pad has to be able to be
described by the Gerber command set.
Just tweak the pad until it is right in orcad.
I am assuming that he is using Orcad Layout, but he didn't use an
uppercase "L" when he used the word "layout".

Obstacles are drawn with lines, thus, they can be represented by
Gerber commands. You need to compensate your DXF drawing for the line
width used in the obstacle definition.

The technique I describe works quite well. In Orcad Layout, you can
import a DXF file to create a PCB max file or a footprint library
file. You can't use polylines, however. After you import the DXF file,
you edit the footprint by tweaking the obstacles that were imported
from the DXF file. The tweaking might be to change the obstacle type
from free track to copper area and adjust the width. You add a small
padstack for your pin so your pad doesn't protrude outside of your DXF
defined area. You associate the obstacle with the pin so it will pass
DRC.

The last four boards I have done all required using this technique. My
BGA packages with a predefined fanout are done using a similar
technique, however, I have a program that spits out an ASCII MIN file
which is converted into a footprint. It's all the same concept.
 
S

SrB

Jan 1, 1970
0
hi frnds...there is the tech fest in NCR region(Ghaziabad)....this two
day program includes many event(approx 40)...also includes more masti
and fun...it includes Robotics..SPICE(OrCad)...VHDL....MATLAB....and
many more..

Win Exciting prizes more that 1 lac....(lots of gifts to every body..)

jst visit on the link
www.rkgit.edu.in


for any query contact to
09873272534
 
M

Marra

Jan 1, 1970
0
hi frnds...there is the tech fest in NCR region(Ghaziabad)....this two
day program includes many event(approx 40)...also includes more masti
and fun...it includes Robotics..SPICE(OrCad)...VHDL....MATLAB....and
many more..

Win Exciting prizes more that 1 lac....(lots of gifts to every body..)

jst visit on the linkwww.rkgit.edu.in

That sounds interesting.
 
Top