Dxf To Board Outline

[JFETT]

Is there an easy way to use an imported dxf file of a
special geometry and convert to the board outline?

[randychase]

I believe one of the new features in release 4 was that you can take a line item and convert it to a board outline. Prior to release 4, the answer is no.

You would need to have the DXF be a board outline first, which is easy to do by the way. Make sure it's on layer board_outline_00

You would need access to AutoCad or Acadlite or such. Create a new layer called board_outline_00 and change the lines to that layer.

It's a good idea to make sure that the lines are one continuous line. In AutoCad, the easiest way to do that is to select a line segment and use the command PEDIT which will prompt you if you want to make a the line into a POLYLINE or PLINE if it is not. Say yes.

Then while still in PEDIT command, type W for Width. Type in .010 and you should be able to easily see now what is a polyline and what is a line.

Still in PEDIT command, type J for JOIN and select all the line segments and arcs that make up the board outline (use the window to select them all).

They will all turn into PLINES also with .010" line width. This should be visually apparent. If they do not, it's because you have overlapping endpoints or the endpoints do not connect.

To fix that condition, you can move the PLINE, which is now one object and see if there are other line bits....or temporarily SELECT with a window and see how many line segments there are.

The easiest way to fix endpoints is to use the FILLET command, type R for RADIUS and type in 0. Then type FILLET again and select the two end points you want to fix. That should make the endpoints in the same exact spot.

A common error is to have a small line segment not attached to the continuous polyline. To deal with that, type ERASE and window around the entire polyline. It should say ONE OBJECT FOUND. If it does, cancel. If it indicates more than one object, type R for REMOVE and select the polyline. Now everything else will be erased.

Another error is the use of ellipses or bizarre segments, like a Polyline that goes to a corner, goes backwards a distance, and then forward to the corner again. That is legal in AutoCad, but may cause problems in PADS. A solution there is to EXPLODE all the polylines back into line segments and then use the FILLET command to return the lines to simple geometries.

[randychase]

Man, that sounded more complicated than it really is. :)

JFETT, what kind of geometry are you talking about? What kind of CAD system was it done on. Is this a complicated board outline shape?

[JFETT]

It was a fairly complicated outline done on ACAD2000.
Your info was very helpfull.

[randychase]

Cool!


Feel free to ask any more questions. I have been using AutoCad since..well..like forever ago. In the very early days of PADS, I used AutoCad a LOT to make odd board outlines and parts. Try making a board outline with a 50 foot radius arc in PADS, but it's a snap in AutoCad.

[ltrakal]

so here is another question about board outline in dxf and cutouts: how do you manage the cutouts? i'm importing from dxf a board outline and this board has a lot of cutouts, do you put them in the board outline layer in autocad and then translate the dxf to the board outline layer in pads?

laszlo

[randychase]

I don't think so. Someone please correct me if this has changed, but a shortcoming of PowerPCB is that you can't have more than one real pcb outline.

So cutouts need to be done with a different layer.

I have created cutouts on the drill drawing layer (including cross hairs for the center or radii) and also thin copper lines (polyline prefered) on the routing layers to act as a routing keepout, and as a guide for the fab house.

[ltrakal]

hmmm, what i'm trying now is to import the cutouts as keepouts in the layer 00, i'll see what happend and write it here..

[tboyer]

Using AutoCad

For PowerPCB 4.0 create your PCB outlines/cutouts/odd details using "2D_LINE_10" layer for example (standard lines).

Create layers BOARD_CUTOUT_00 AND BOARD_OUTLINE_00.

Draw your polyline with a width defined using the BOARD_OUTLINE_00 layer. Make sure the line is unbroken and closed. You can define arcs as needed.

Draw another polyline with a width defined within the board outline using BOARD_CUTOUT_00 Layer. Make sure the line is unbroken and closed.

While drawing the polylines you can use the 2D_LINE_10 to snap to intersections to make it easier to draw the polyline.

Hide your 2D_LINE_10 Layer.

Make a block. select both polylines and name the block BOARD_7.

Unhide your 2D_LINE_10 layer.

Save as a DXF selecting only the board drawing you have completed.

If you have a coordinate error, you can dxf out a default PCB file to start the work with.

Using AutoCad and these type of techniques you can also design inductors, coils, odd shapes, and RF geometries.

[ltrakal]

well this is how i am doing the board outlines now but why make a block? can you explain that please?
see i found a problem...what i did is i made a board outline and a cutout inside and i dxf it out from power pcb...so i have two very important layer names board_outline_00 and board_cutout_00.. so i started from scratch in autocad to make my board outline and cutouts in the correspondant layer...the thing is when i go insde power pcb via dxf the cutouts are not being select when i select a board outline, and they should... why is that?

[tboyer]

I reverse engineered a PCB board outline with a cut-out. The output DXF from PADs grouped the cutout and board outline layers into a block called BOARD_7. I exploded the block and I got both board outlines as seperate layers.

Well after finding this out I went through the process I listed above and imported it into PowerPCB. If you do not create a block PowerPCB will not combine the layers into one board outline.

You must make a block.

[tboyer]

I did not try the process above from scratch. Maybe you have to export a sample board outline with a cutout and work from that file making sure that the block name matches. I have not experimented that much with cutouts yet. If you no not have a cutout the process does not need to use a block.

[ltrakal]

you are right, it must be a block so what i did is i imported the board into dxf, modifed the block in autocad, added more cutouts and save it again but when i want to go back to powerpcb i can't even load the file, i have an error and the program quits itself....

[tboyer]

Added more cutouts???

I have not tried multiple cutouts yet. Make sure your block's "INSERT UNITS" is "UNITLESS". assigning inches or anything else will crash Pads. Well in any case, any time Pads get a dxf command it does not understand it crashes.
If you programmers are listenining "THERE IS SOMETHING CALLED A GENERAL ERROR HANDLER", PLEASE USE IT NEXT TIME.

Look! try this. Create a simple sample of your board in Pads that includes all of your cutouts. Do not worry about dimensions, just make sure the entities are there. Export to dxf and open the file in AutoCad. Study the block name. Explode the block and look at all of the cutouts for thier names.

Delete the board in the file and then recreate your board using the information you gathered from the original.

[ltrakal]

MAN I'M GETTING CRAZY!!!!!!!!! i did that already, the multiple cutouts inside the board outline are just polylines in the board_cutout_00 layer, so what i did was in autocad just a drawing with 2 cutouts, there is an error when i get into pads saying that the cutouts are intersectiong the board outline..

[tboyer]

Can you e-mail the Auocad file to me. I will look at it and tell you whats wrong. tboyer@cardiacscience.com

[tboyer]

By the way when makeing the block make sure you are in layer 0.

[ltrakal]

yeaph i'm in layer 0

[randychase]

^

[tboyer]

Attached is the PCB file I created that shows the multiple
cutouts. You can DXF out and load into AutoCad to
determine its structure.

[randychase]

Thanks, I find this to be one of my most useful threads. I keep coming back when I forget what layer name to use. :)

[tboyer]

Pads or now Innoveda had a Technical Application Note on this.

I have the copy but it is not in electronic form. One of these
days I will probably take it home to scan and convert into
PDF. There are most likely some changes since V4.0 allows
more than 20 layers.

You can call Innoveda and ask for the APP. Note or wait
until I get to converting it.

The Name:

"Issue: Creating a File in ACAD V13 & V14 only, and DXF the
information to PowerPCB using the PADS DXF translation
option."

Happy Hunting:)

Tim

[Franco]

Didn't find the app note on innovedas site.
Had anybody more luck?

It would be nice to have a dwg/dxf template file with all layers etc. @ pcbstandards

[randychase]

Originally posted by Franco

It would be nice to have a dwg/dxf template file with all layers etc. @ pcbstandards

Just saw this. Excellent idea.

[dmichalo]

I am trying to convert an AutoCAD file containing the board outline into PADS. I have made a layer called board_outline_00 and moved the joined-closed polyline to that layer. How does that get into pads as a board outline. I followed the steps in this thread as far as it will take me but need the rest. Please help.

[randychase]

You need to output the file as a DXF. SAVEAS. I use DXF Release 14.

Then in PADS, import the DXF file.