Inventor DWG interoperability between Inventor & AutoCAD

[Anonymous]

Guys,

We have developed full bus models & drawings in Inventor for our clients and now they want use inventor drawings to create their floor plans in AutoCAD. I was thinking of making use Inventor DWG which can be opened in AutoCAD, but it looks we can only annotate with this file, almost seems like interoperability meant one-way from AutoCAD to Inventor only. I badly want to maintain model link back to Inventor, but it looks we have to break since they want to do it in AutoCAD and not in Inventor (since they don't have expertise in-house).

Any suggestions would be welcome!

Thanks,

Arjun

[phaeronkor]

Hello, Arjun

What's the problem to save Inventor drawing to AutoCAD DWG file? It will be fully editable in AutoCAD.

File - Export - Export to DWG

[mflayler2 · Accepted solution]

The Inventor views can be referenced directly into AutoCAD by use of Design Center (type ADCENTER in AutoCAD, browse to the Inventor DWG and look at the blocks in the file).  When an update happens in the Inventor DWG, you do have to right click in the Design Center and choose to reload the reference.  They should not change the geometry from the Inventor views because YOU own that data to change.  If they want the ownership to change the file, then they need to learn how to use Inventor or they have to be okay with a Saved off un-linked DWG of the Inventor drawing.

If you want FULL associtivity you need to use Factory Design Suite which will sync back and forth with Inventor and AutoCAD.

[Anonymous]

I'm trying to keep the model reference. AutoCAD DWG would lose the reference.

Arjun

[Anonymous]

Thanks Mark! I tried your method as you described, but the ADCENTER is unable to insert Inventor DWG blocks where it has no issues inserting the AutoCAD DWG blocks. Am I missing something? See attached. 

Thanks,

Arjun

[mflayler2]

Filled-1 is not a valid block.  Try it with the others but use a right click on the block in the design center.

[Anonymous]

Same on the other three view blocks too. I've attached the Inventor DWG file for.eg which I'm trying to insert, see if you get the same issue.

Thanks,

Arjun

[mflayler2]

The functionality works fine on my end, but I do not have your models.  I tried it with one of my Inventor DWGs and IPTs and it works fine.

Make sure you have the models and drawing in the same directory and that you do not have Inventor open at the same time.

[Anonymous]

Mark- Are you inserting it in the same Inventor DWG file in the model space (which I've been able to do ). I have been trying to insert it in a new drawing, since I would to have assemble the different systems like floor, steps, roof & sidewalls etc.

Thanks,

Arjun

[mflayler2]

I am inserting the views into a new AutoCAD drawing using Design Center to reference the Inventor DWG file.  That is the functionality at play here.

If that is not what you are trying to do, please explain your process in more detail.

[Anonymous]

Mark, 

Sorry I'm not able to get this to work. Please see attached. I'm trying to insert WB-0002501 drawing views through Design Center into Sample.dwg file to no avail. If this works then I can replicate the process for the floor plans.

Thanks,

Arjun 

[mflayler2]

Something is corrupt in how you created that Inventor DWG.

I had to create a new one and it worked fine when I place it.

[Curtis_Waguespack · Accepted solution]

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@Anonymous wrote:

Guys,

We have developed full bus models & drawings in Inventor for our clients and now they want use inventor drawings to create their floor plans in AutoCAD. I was thinking of making use Inventor DWG which can be opened in AutoCAD, but it looks we can only annotate with this file, almost seems like interoperability meant one-way from AutoCAD to Inventor only. I badly want to maintain model link back to Inventor, but it looks we have to break since they want to do it in AutoCAD and not in Inventor (since they don't have expertise in-house).

Any suggestions would be welcome!

Thanks,

Arjun

---

Hi June89,

If I understand correctly, you can just insert the views in your Inventor DWG as AutoCAD blocks, directly from Inventor. Note that for some reason Inventor only allows one block in ModleSpace at a time.

Maybe you would do this on a new sheet? And then the client can use that sheet as needed. They can explode the blocks and do what ever they need to. But your Inventor views are protected from the AutoCAD user.

Opening the file in AutoCAD as  Mark_Flayler, mentioned might give you a bit more control though.

Note that you can create Xrefs of those blocks as well, which allows for some interesting "live linked" workflows. I show some of that at this link, although the video there is a bit of a different workflow, since it's sort of round tripping from Inventor to AutoCAD back to Inventor:

http://forums.autodesk.com/t5/inventor-general-discussion/drawing-views-of-dwg/m-p/6431519#M604151

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[ChrisMitchell01]

See this article:

https://knowledge.autodesk.com/support/autocad/learn-explore/caas/CloudHelp/cloudhelp/2017/ENU/AutoC...

You should be able to create associative views of Inventor data without the need to use blocks or exports, etc.

I haven't tried this for a long time but the last time I used it in AutoCAD Mechanical it worked just fine.

Hope this helps,
Chris

[Anonymous]

I save an Inventor dwg.

Open the dwg in AutoCad.

Change the dwg in inventor & save.

The blocks can be seen in autocad design center but the option to refresh is greyed out..

If I close & reopen the block is updated - can the refresh be forced keeping the drawing open?

Thanks

Andrew

[jeffsteiger6735]

Old thread I know, but is there a way to bring in Inventor drawing data complete with annotation, into an Autocad drawing?

I have an Inventor IDW where I have a hole table to call up 250 or so base plate anchor positions with leaders giving a unique identifier to each anchor plate. We then have an Autocad (mechanical) drawing that later would use this same model information AND the anchor plate identifier annotation as reference to help relate some additional equipment.

I've tried the design center method which works great (except for the fact that I have to create a "saved as Inventor DWG" duplicate file) for keeping the model data linked, but it doesn't seem to be able to bring in any of the IDW annotation.

[johnsonshiue]

Hi Jeff,

I think saving as Inventor dwg should work. The annotations should be editable in AutoCAD. Could you share an example here? Another option to consider is simply create associative drawing views in AutoCAD. I am not sure if you are aware of VIEWBASE command in AutoCAD, which can create associative drawing views to Inventor components. Then you can use drafting tools in AutoCAD to add annotations.

Many thanks!