DipTrace Forum
http://www.diptrace.com/forum/

How do I make IPC-7351C rounded corner pads?
http://www.diptrace.com/forum/viewtopic.php?f=5&t=11448
Page 1 of 1

Author:  jbeng [ 20 Feb 2017, 22:57 ]
Post subject:  How do I make IPC-7351C rounded corner pads?

According to at least one online source, IPC-7351C recommends that most SMD pads be made as rectangles with rounded corners. Not rectangles with pointed corners and not "ovals".

:?: But how do I specify those in a DIPTrace pattern?

So far, I have drafted using ovals for elongated pads on QFPs etc. and rectangles on more squarish pads such as chip resistors, but that is obviously just a compromise that hasn't been production tested.

Author:  Tomg [ 21 Feb 2017, 16:18 ]
Post subject:  Re: How do I make IPC-7351C rounded corner pads?

To date, DipTrace does not offer a rounded-rectangle template for pads in the Pattern Editor. If you know the exact dimensions, here is a work-around...
1) Draw the desired pad outline in your favorite 2D CAD program and save it as a DXF file.
2) Click on Pattern in the Main Menu of the Pattern Editor and select Import from DXF... in the drop-down menu.
3) In the Open dialog window navigate to and select the DXF file and then choose Open.
4) In the Import DXF dialog window set DXF Units: to match the DXF file setting, Import Mode: Add, select/highlight the appropriate layer, set Convert to: Top Signal, enable the [X] Fill Closed Areas option and click on the [Import] button.
5) Right-click on the outline of the imported object and select Convert to Pad in the pop-up menu.

Author:  jbeng [ 26 Feb 2017, 14:37 ]
Post subject:  Re: How do I make IPC-7351C rounded corner pads?

After searching for a DXF editor and trying to create a rounded pad for a typical 0805, I ended up with the simple DXF file below which provides the shape as a closed polyline.

However when I imported it in the pattern editor, it converted it to a polygon with each of the corners as 6 line segments (1 per 15 degrees), not to the elusive "shape" object found in some patterns. Some of the other DXF files I tried caused access violations in the pattern editor (the first ones I actually encountered in DIPtrace, so it is still more stable than it's old reputation :) ).

So as a temporary approach, I just input that polygon directly as a pad specification, which is not completely correct (it will probably become a polygon shape in the Gerber output too), but closer to the ideal.

(I apparently cannot attach DXF or txt files in this forum, so here is the DXF pasted in as text):

Code:
  0
SECTION
  2
HEADER
  9
$ACADVER
  1
AC1014
  9
$HANDSEED
  5
FFFF
  9
$MEASUREMENT
70
     1
  0
ENDSEC
  0
SECTION
  2
ENTITIES
  0
LWPOLYLINE
  5
100
100
AcDbEntity
  8
Layer_0
62
     7
100
AcDbPolyline
90
     8
70
     1
10
-0.44
20
0.52
10
0.44
20
0.52
42
-0.414213562373095
10
0.69
20
0.27
10
0.69
20
-0.27
42
-0.414213562373095
10
0.44
20
-0.52
10
-0.44
20
-0.52
42
-0.414213562373095
10
-0.69
20
-0.27
10
-0.69
20
0.27
42
-0.414213562373095
  0
ENDSEC
  0
EOF

Author:  Tomg [ 26 Feb 2017, 16:02 ]
Post subject:  Re: How do I make IPC-7351C rounded corner pads?

You can attach a zip folder with your *.dxf file inside. I was able to copy your text over to a text editor and save it as an unspecified file type. Then I added a *.dxf extension to its file name and imported the new *.dxf file into the Pattern Editor without a problem. The illustration below is a partial screenshot of the imported figure after it was converted to a pad. I tested the new pad in the PCB Layout editor and I also examined it using the Gerber Preview tool. It looked fine there, too. By the way, the polyline drawing figure is the norm for DipTrace. To date, DipTrace cannot import splines.

p.s. I attached a zip folder containing a file named "pad.dxf" that was created using your text.

Author:  Alex [ 27 Feb 2017, 03:39 ]
Post subject:  Re: How do I make IPC-7351C rounded corner pads?

We consider new IPC-7351C standard. At the moment DipTrace doesn't support rounded rectangle pad shape but we will try to add them in future. Until we implement new pad shape, you can use oval or polygonal pads (depending on pad length and width).

Author:  jbeng [ 10 Mar 2017, 21:10 ]
Post subject:  Re: How do I make IPC-7351C rounded corner pads?

Tomg wrote:
You can attach a zip folder with your *.dxf file inside. I was able to copy your text over to a text editor and save it as an unspecified file type. Then I added a *.dxf extension to its file name and imported the new *.dxf file into the Pattern Editor without a problem. The illustration below is a partial screenshot of the imported figure after it was converted to a pad. I tested the new pad in the PCB Layout editor and I also examined it using the Gerber Preview tool. It looked fine there, too.

:mrgreen: Looked fine here too, but I presume it won't be converted back to Gerber arcs (G02/G03) or AD code 1 circle primitives.

Tomg wrote:
By the way, the polyline drawing figure is the norm for DipTrace. To date, DipTrace cannot import splines.

:geek: RS-274X2 Gerber only supports lines and circular arcs, not splines. At least as far as I can tell from the 2016.12 spec. :idea: Section 4.13.4.1 contains a handy macro for representing these pads as flashable apertures.

Anyway, some predefined DIPtrace patterns do include actual arcs as part of "shape" objects, at least in non-copper layers, but they don't seem editable in the current UI.

Page 1 of 1 All times are UTC - 5 hours [ DST ]
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group
http://www.phpbb.com/