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Autocad 2D to Pro-E solid model



I design simple circular shapes in 2D AutoCad. I would like to be able to send these drawings to Pro-E so we can write tool passes for our CNC machining center. What is the easiest and most affordable way of getting a 2D drawing into a solid model?


New member
Import to the Pro/E sketcher...

Hello andy81563,

I would import each profile into a Pro/E sketch and then use the sketch in Pro/E to create the solid feature such as extrude, revolve, sweep, etc. Be sure to validate the geometry in the sketcher. Sometimes inported 2D geometry can leave gaps where line or curve segments are supposed to connect.

Good Luck.
3DCADTips Help Desk :cool:


you may evev try AUTOBUILDZ for proe. this is good enough for simple components.


2d programming in proe

I assumes that u want to import 2d sketches in to proe and do the programming insted of going 4 3d .
the best way is open ur 2d autocad sketch in proe as a part file (it is possible) and assemble that part to pro/mfg, and do tool paths by u sing trajectory milling,
But by this way u wont get associativity and u wont b able to do any kind of pocketing operation, only contouring.


AutoCAD to Pro/E Solid Model

In Wildfire 2.0, you can initiate a feature (say, extrusion) and when sketcher opens - "place section" and hit the file type drop-down and select ".dwg" to pick your ACAD 2D file. You can then extrude the geometry. As I recall - you first have clean up the 2D .dwg so that it includes only the geometry you want to use for your geometry profile (in ACAD or UStation). If you don't - Pro will give you a warning about taking a long time to import the section and your computer will hang, etc. Not good.



There are three ways of importing 2D drawing from AutoCAD to Pro/E.

1. Open a new part file. Activate any skectch feature command you need e.g. extrusion. Go to the sketcher and click on manu bar Sketch->data from file, locate the dwg file of AutoCAD and click ok (don't forget to change the filter to dwg). you will have to tell the position and scale for the sketch and job is done. you can modify the sketch if you want to. The problem in this way is that Pro/E applies the constraints automatically which, most of the times, changes the profile.

2. Open a new part file. Click on the manu bar insert->shared data->from file, change the filter to dxf and locate the AutoCAD file (make sure that you have saved the file in dxf in AutoCAD), click ok and then you will have to select the coordinate system, you can select the default as well as a new coordinate system. Now any section or any line/curve of the sketch can be used in the new feaures. Use-edge command will be used in the sketcher mode to select the sections. The problem in that way is that you can not edit the profile once you have imported it in Pro/E. But if your profile is final in AutoCad then this is the best way to work.

3. Use AutoBuildz if you have simple sketches and parts.

Make sure you are using wildfire 2.0 version of Pro/E. AutoCAD 2004 works fine with that version. The AutoCAD filename should not contain any special characters like , . ; ' & spaces or you will not be able to locate the files.


New member
2d to Pro/E

Save the 2d view out from autocad as dxf. - Import that into a drawing into Pro/E WF2.0 - export from Drawing as IGES with respect to a specific CSO (coordinate system) - import IGES into Pro/ENGINEER with respect to a specific CSO

Do the same for each conscutive view each with a separate CSO so everything lines up.

Then you use the regular Pro/ENGINEER tools to model your product.