How do I import an assembly from AutoCAD into Inventor?

[betaphase]

Hi All,

I have a question about compatibility between Autodesk AutoCAD and Autodesk Inventor. What is the best way to import an assembly from AutoCAD into Inventor (such that I can transfer over the maximum amount of geometric information, import parts as individual part files and keep the part names, etc.)?

I'm an inventor user and have recently started working at company where most designers have been useing AutoCAD. They've been creating 3D models and assemblies using the 3D functionality in AutoCAD, and I'd like to be able to work on these older projects in the environment I'm most familiar with. I've been importing the AutoCAD assemblies into Inventor, but there seem to be some limitations that I'm hoping I can circumvent. I've done this by opening the AutoCAD file and selecting the option to import, and trying out several options through the import dialogue boxes.

I've noticed that I'm able to import each component as an individual part, however, the original part names are not maintained. Furthermore each part does not seem to have geometry that you can actually edit. The way I've worked around that so far, is to individually open and save each imported part with an updated file name, but ultimately that's only useful for parts that I don't need to edit. If the original file requires any changes then I just have to draw it again from scratch.

I've also tried importing the assembly as a single part, and I've noticed that now each part is saved as an object with the proper part name, however I'm not sure what to do with the file from this point and/or how to turn that into an assembly.

I noticed that the import dialog boxes include an option to "import into repair environment" or something along those lines, but I'm not familiar with that process.


Is there a way around these limitations? If so what are the steps?



Thanks very much for your help,


Bruno

 

[mcgyvr]

lots of info here..

http://knowledge.autodesk.com/suppo...9996B399-313F-4AC2-9E39-B92CE5112F30-htm.html

and here

https://screencast.autodesk.com/main/details/142eca92-7f90-44ff-bb4b-b3e3f819aeab

 

[betaphase]

Hi Mcgyvr,

Thanks very much for your reply. I'd actually already been looking at that first link you pasted, and I also just watched the video from the second link. I don't think these cover the two questions I was most interested in.

- Can I import a .dwg into an inventor assembly while maintaining geometric information that I can edit?

- Can I import a .dwg into an inventor assembly such that objects are imported as individual part files and with the original part names, etc?

I've tried following the outlined steps from your links, and also experimented with different import settings, but it doesn't look like this is possible.

Thanks all!

-b

 

[mcgyvr]

There is no history/feature tree in Autocad but getting a 3d "solid" from an autocad file should be covered in those links and any solid can be edited with the tools in Inventor. (no different from opening a step or iges and editing it.. feature tree is missing but you can still make changes)

as to the original part names question.. I have no idea..

I'd NEVER work from Autocad "3D" garbage no matter what I have to do.. I'd just remodel everything properly in Inventor.. NO WAY would I want to use Autocad geometry for any product I need to support/update in the future..

 

[betaphase]

I understand. I was hoping that the software packages would possibly be compatible enough to avoid having to remodel everything.

Thanks very much mcgyvr. You've been very helpful.

Best,

-b

 

[mcgyvr]

Don't get me wrong..
You can easily use the 3d dwg files and depending on complexity you might want to do that..
But personally I'd much rather know I was working and moving forward with 100% easily editable/feature tree based geometry if I was moving out of the autocad 3d stone age..

 

[betaphase]

Thanks Mcgyvr. I completely understand.

The only problem is that I'm working with a lot of legacy designs from AutoCAD (3D). sometimes my assignment may be to make a few small changes to an existing design and get the project into production asap. So at that point, I can either import to inventor and try to keep as much original work as possible, remake everything from scratch, or just get better with AutoCAD and keep working "in the stone age" as you put it.

 

[betaphase]

One more question though, Mcgyvr. In your reply above you'd written " feature tree is missing but you can still make changes". How do you mean that you can still make changes?

For example. Something as simple as a part made of tubing. I can't import it and then change it's length. There is no parameter to change. I can theoretically create a sketch on one end/face of the tubing and extrude that further, but that isn't really practical when you have chamfers, threading and so on, and would be even less straightforward for other parts. No?

 

[Sparweb]

A few suggestions - I don't know how practical they will be for you:

Direct Edit in Inventor. This allows much more powerful manipulation of the faces of a solid body, even if it comes from imported geometry.

Multi-body parts in Inventor. An IPT file can have multiple separate, distinct bodies in it. I frequently create multi-body parts, for many reasons. In your case, the individual bodies can be split as separate parts and built into a single assembly - all in one dialog box. Find it in Productivity Tools. None of the parts will have constraints - they'll all be grounded. Expecting proper constraints on imported geometry is a bit of a pipe-dream, but there are new contenders in the 3D parametric design world taking a shot at it and have a chance. But not Inventor. Anyway, you can un-ground the parts and constrain them as you like in the assembly later.

The example of the tube you must shorten/lengthen while preserving its end fitting features: There are many ways to approach that problem. Some will leave more parametric breadcrumbs to follow when editing the part later. One way would be (after importing to IPT) to create a plane to slice the part in two pieces, chop out a segment of tube with Extrude, then replace the lost material with a new solid. The dimension of length of that new "middle" piece of tube is parametric now. The end of the tube (floating off by itself) can be moved to conjoin to the new length of tube with a Direct-edit of the Body. The amount the body moves in the direct-edit is also parametric, and a brief formula can relate the dimension of the new piece of tube with the relocation of the tube end fitting. That way you can change one length, and the other brings the end fitting in place. Voila, shorter tube, same end features, no gaps.

There's another way to go about this, starting in AutoCAD before you import (more boolean operations, but the same "Slice" concept) that could also work.

Ultimately, you won't really be in control of the Inventor models until the entire model is built parametrically.

STF

 

[mcgyvr]

It addition to what SparWeb has already stated there is also feature recognition which "attempts" to rebuild the feature tree..

https://apps.autodesk.com/INVNTOR/e...e.exchange.autodesk.com:FeatureRecognition:en

but yes.. there are no parameters/feature trees but direct edit/new sketch,etc.. can allow you to modify non-native parts.

 

[betaphase]

@Sparweb, Thank you so much for your reply. That is very well thought out, and I'm sure it will help me in the future. I have to admit I'm not sure I'm familiar with using "direct edit" but I'm just looking into it now, and it looks like it gives me some options. The approach of using multi body parts and then recombining them in the productivity tools should also be very helpful. I'll definitely have to experiment a bit with all that.

@mcgyvr, Thanks again very very much for your continued help. This is exactly what I was hoping for.

Thanks all. Now I just to figure out if it's more worthwhile for me to use all these work-arounds, or just model from scratch/just learn AutoCAD.

Cheers,

-b

 

[Sparweb]

Try to learn them both! It's like having a hammer and a chisel.
You can do lots of things with either one of them alone, but imagine the sculptures you can create when you use both of them together!

STF

 

[betaphase]

Haha. That's the plan...

Thanks again,

-b