SIMPLE WAY TO BRING COMPLEX GEOMETRY INTO SKETCH ?

[proedesign]

I have to bring in the company logo (complex splines geometry) in to sketch mode to place it on surfaces and extrude it out. The file that I have for the logo is an iges and every time I bring it in to sketch mode I have problems because it takes too long to redraw and regenerate due to the fact that Proe dimensions for me every segment of the logo.



Is there a way to make the logo as one entity or something like that so, when I bring it in to sketch is small size geometry and all I have to do is scale it to the correct size?



Thank you all,

ProG

gonzalo@proedesign.net

 

[adicar01]

try dxf format, you must take care at scaling model after import.



adicar

 

[bhayden]

Would turning off intent manager prevent the auto dimensioning?



Bernie Hayden

XKL LLC

 

[ProFishent]

Why don't you bring it up once in sketcher and and save the sketch. That way you only have to dimension it once! Then you can place it, and scale it to any model you want.

 

[tarundeep]

Dear Pro G

Take the IGES file in the DXF format and scale it accordingly.The DXf format then can be taken into the file and you can have scale of your choice.

 

[Huug]

Hi,



Getting logo's on solid parts is always tricky.

As a designer of several plastic parts for different customers I have faced the problem many times.



The problem is that imports often translate the curves to too many segments, which causes trouble in sketcher.



I'll describe the method that works the best for me, allthough it sounds complex.



The import file of your logo should be in the form of a 2D IGES curve.

If you don't have it, create it by exporting a ProE drawing with the logo of the correct size. Don't forget to blank the format.



In your part, create an offset coordinate system.

Import the Iges to the new Csys.

Position the import by modifying the dimensions of the Csys.

Then sketch a datum curve over the import. Use the intent manager and select several points as references of the first caracter of the import. Sketch a spline through the refererred points. The more points you selected, the better the spline follows the import.

Continue with another sketched curve for the next character. As the import has straight lines, you can use edge. Don't try to capture the complete logo in one sketch.

When finished creating the skecthed curves over the logo, blank the import by layer.

Now use the sketched curves for protrusions, cuts, offset surfaces to generate the desired volume of the logo on your part.



Good luck!



Huug

 

[kyle88]

ProG,

I too have battled the company logo problem here. The easiest (and flashiest) way that I've come up with is to create the protrusion in any way you would like. Then create a UDF with the protrusion. With a UDF you have the option to blank the dimensions so they will never come up. Don't worry about scaling, you have that option to scale when you are placing the UDF. As a side note. If you use curves when creating the protrusion. Make sure that you Use Edge as you normally would to get the geometry, then go to your Section References and break the reference to the curves. This will take a LONG time (3-4 min.) for Pro to generate the dims and you will think that it locked up, but it will get done. Remember you only have to sit through it once. If you are putting the logo on a curved surface this can be done to, with draft? No problem, but this reply is too long as is. E-mail me if you need it (kyle88@juno.com).



Hope this helps,

Kyle Davidson

RACAR Intl.

Anderson, IN