How to access "File -> import" in ProE2001?

I am unsure of exactly what you are trying to do. I have found the best way to use a dxf file, is turn the intent manager off, insert the sketch,zoom in as much as possible, and then auto dim sketch

cheers

Hello Craig,

I am new to ProE so could you please give me some more details about what should I do?

I turned off the intent manager, but then I lost the tool for bring in the geometry from a .dxf file.

Second, problems with scaling, changing geometry in sketch mode may be due to the way the dxf was saved. Sketcher does, however, place a scaling box in the window with the sketch so that you can adjust scale, plus the sketch comes with drag, rotate, and rescale handles that can be used to move and fit the sketch.

Third, you can 'import' geometry into a part with 'Insert>Shared data'. There are many types of data that are reusable in Pro/e. The 'From file' option is probably the closest thing that's left of an import function. With dxf, though, it doesn't give you any control such as you've asked for, over scale and it imports drawing data as simple 2d entities, without dimensions.

Fourth, if you are using the dxf for a base feature, you can simply open it from the 'File>Open' menu. By default, this menu funtion highlights .prt files, but many others are available. The box labelled 'File type' has an arrow to the right which opens a drop down list of all the files Pro/e can open. Scroll down until you find dxf in the list and open from here. See if that is more like the functionality you were looking for. There are several ways you can open a dxf, depending on how it was created. Not all those offered may be appropriate, so you may have to experiment. This is, however, a little more flexible than the sketcher functionality. BTW, I'm using Wildfire, starting to forget 2001 already, so hopefully this is on the mark.

David Janes

Hello David,

The problem I had was not with the scale of the geometries I try to bring into proe from dxf file, rather whatever method I use, proe would impose dims on those geometries and sometimes alter the relationships between some of them (seems proe would make some assumptions ahout the relationships).

What I would like to know is that if there is a way to bring those geometries into proe as what they are without proe doing anything to them. I would afterward put dims and relationships to them. This way I could have full control.

Thanks for your help.

David Janes

relationships).

Hi David,

Yes, I tried one of the methods you mentioned above and is successful (import geometries from dxf file directly into a part then construct a new sketch based on the imported features using "create entity from an edge" tool). Thanks.

Best regards,

Geoffrey

: : Hi David, : : Yes, I tried one of the methods you mentioned above and is successful : (import geometries from dxf file directly into a part then construct a new : sketch based on the imported features using "create entity from an edge" : tool). Thanks. : Glad to hear SOMETHING worked. But if you are going to be doing a lot of this 2D to 3D work in the future, may I suggest you try this *free* software from PTC:

This is the problem everyone is trying to solve: how to get from legacy 2d to 3d solids. There's got to be an easier way and it looks like PTC is working on it.

David Janes

Bummer. Only works on Wildfire.

I am in the process of downloading it from PTC. Would be a shame if it works only with Wildfire.

Geoffrey

: > Bummer. Only works on Wildfire. : >

: >

: : I am in the process of downloading it from PTC. Would be a shame if it works : only with Wildfire. : Well, I guess I'm going blind or I just forget that not everyone has Wildfire, because Dave's right. The link I included above does say that it's a plugin for Wildfire. I knew it was a new functionality but it never occurred to me that it would be exclusively for WF. Sorry for the miscue. One more thing to look forward to when you upgrade.

DJ

Do'nt get your hope up on this... at the moment you're better of building your 3d model from scratch.

but it has potential.... maybe within a few releases....

Greets

See the reply to the thread "Re: Problems using dwg file as a base part rel

2001" above from Jeff Howard.

You can avoid importing the entities into sketcher if you create a 2D IGES file of the enitities, and use that as a base part. ProE treats these entities as a block of lines that it doesn't have to calculate, yet you can still reference them to create solid and cut protrusions. Much quicker than Sketcher, but you cannot modify the dimensions of the section.

also check out the new config.pro option sketcher_import_exact_geom See:

for more details