importing auto cad sketches

[ivan sosa]

Hi everyone! I hope the day is great for all.


I am into making solid models of asome plates like the one I show in the first image. As you see tje lines 1, 2, and 3 are at an angle. Theese plates are drawn in autocad. I am using a procedure of saving them as *.dxf files, start a drawing in pro-e (2001i) pick insert\data form file...save and use that as my sketch profile for my solid modeling.


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The problem is that with the intent manager on pro-e makes some of them hoixzontal and some of them vertical as in the second image. If I turn off the intent manager I cannot pick SKETCH\DATA FORM FILE to open the file as a sketch. Is there a way to make pro-e take such a sketch as final for a protrussion? Thank you for your time.


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[puppet]

try importing that data as a part, rather than a sketch
then put that feature on a different layer, then sketch over it. or use the offset button.

 

[brchapman]

You can jump through the hoops required to import the AutoCad data and use it in sketcher mode but...You will probably find it easier and faster to create the sketch in Pro/E. If the geometry seems to complex, than break it down into several simple sketches rather than one large complex sketch. You will find you will have the plate modeled with the geometry you have shown in 5 or 10 minutes.

 

[ivan sosa]

Thanks. I will try both your ideas. I have about 16 of theese to model.

 

[DEAMER]

Try saving your file as a DWG and importing directly into sketcher.


I do this all the time with odd shapes and have no problems at all.


Regards,


Todd

 

[mechanical01]

you can also import ur geometry as IGES into partmode directly. I did this often and find it successful. The above two ideas will work also.

 

[puppet]

if u have simple geometery then u can import into sketcher very easily, But when its complex... and intent manager starrts struggling and moving things around. then its best to import as a part. it creats a flat 2d datum curves of your object. then you can easily use the offset.

So it really depends on how complex ur geometry is. Also its its very easy stuff just redraw it.

 

[ivan sosa]

When importing the dwg format drawing by inserting data in a drw file started with this purpose and then using that as a sketch on a prt file when the sequence of commands "feature-create-solid-protrusion..." demands to start sketching I noticed that as far as the dimensions remain "weak" the shape of the sketch is kept just as it is in auto-cad. The distortion comes when you accept the sketch as final using he check mark icon to specify the thickness of the extrusion. What I did was take the weak dimensions -either one by one or with a window to take a bundle without picking any of he lines that form the geometry- , right clicked on them with the mouse and chose the "make strong" option and guess what! The shape is kept.

This occurred to me when I started trying brchapman's suggestion.

Thanks.