Problems importing .DXF or .DWG files into Inventor

[Anonymous]

Hi, 

       I am trying to import a .DXF or .DWG file into Inventor, either as a new drawing or as a new part, but the files are failing to load. I have checked in DWG Trueview, and the image is loading and is correct, but it is no loading in Inventor. The drawings are of terrain map contour lines which have been converted from .SHP and .SHX files. The DXF is 1.9mb and the DWG is 648kb, but neither will load. Any ideas? Many thanks for your help in advance!  EB

[JDMather]

What version of Inventor are you using?

What are your -dwgunits in AutoCAD?

Can you describe what you want to do with this geometry in Inventor?

[Anonymous]

Hi, 
      Thanks for your response.  I am using 2018 Professional. 
Kind regards.

[Anonymous]

I am trying to extrude the contour lines at different heights to make a 3d map.

[JDMather]

Autodesk had products specifically for topos.

I don't think you will get very far with Inventor on this project - not the right tool for the job.

Perhaps if you could simplify the dwg by removing at least 50% of the geometry.

[johnsonshiue]

Hi! Instead of importing the dwg file as sketches, there is a better workflow to use, called DWG Underlay. Start a new part -> Create -> Import -> pick the dwg file and pick XY plane and the origin point. The DWG geometry will be linked to Inventor. To create body geometry, you can create a sketch on XY plane. Then use Project DWG Geometry command (click the downward arrow in Project command) to project the DWG geometry to the sketch.

This workflow was introduced in Inventor 2016 or 2015. The point is to associatively link to DWG file and bring in the geometry quickly. The user can selectively project geometry from DWG to a sketch. In the past, the import DWG workflow tried to convert all geometry to compatible Inventor geometry. It takes a long time and it can fail if somehow the geometric definition is ambiguous.

Please try this workflow and see if you get better result. I just tried it and it seemed to work fine for me. Like JD mentioned here, the key question is what you really want to do with these contour. Inventor is very good at geometry meant for manufacturing physically. If the geometry is not for manufacturing, the options and workflows will be limited.

Many thanks!

[harrelsontrumpets]

Wow! I'm really surprised to learn that Inventor is so very limited concerning dxf imports. I'm trying ti import a simple 2d sketch and, after hours of attempts, I'm giving up. It seems the simplest of tasks can be too much for this powerful software?

[JDMather]

Attach your dxf file here and someone will show you how. 

So easy to get help!

[harrelsontrumpets]

It has not been easy. I have asked numerous times and watched every video I can find on the subject and the file still does not import properly. Please do not belittle my issue without having direct experience with my application. I've attached the file for you to show me your magic.

[JDMather]

What version of Inventor are you using (including Service Pack/Update information)?

There  was an issue 2 or 3 releases back that required an extra step.

Give that the geometry has Z coordinates - import as 3D sketch that you can then Project Geometry to a 2D sketch.

[JDMather]

Any news on what version of Inventor you are using.

I can create a video, but it would help if I knew what version of Inventor you are using?

[johnsonshiue]

Hi! Do you have the file in AutoCAD dwg? If yes, you can use DWG Underlay workflow to bring in the geometry to Inventor. In Inventor, start a new part. Import -> pick the dwg file -> pick an origin plane and the origin to place the dwg as an underlay. Then you can create a sketch on the same plane and then use "Project DWG Geometry command to project the dwg geometry to Inventor sketch.

Many thanks!

[Anonymous]

Thanks Johnson, I would have never figured this out myself. I'm having to use this method a lot for importing 2D .dxf or .dwg flat patterns and it works flawlessly everytime!

[engin.tosun]

Hi I am having an issue with importing dwg file in Inventor.  I am using 2021 version Inventor but it either doesn't load the dwg file or make mistakes when uplading dwg file. Is there a practical way to open dwg file without mistake or failure.

[johnsonshiue]

Hi! The issue does not sound the same as the original thread. Please share an example dwg file here or start a new thread. You can also send the file to me directly johnson.shiue@autodesk.com. I can take a look to understand the issue better.

Many thanks!

[engin.tosun]

Thank you Johnson,

I will send the 2 files in to your email address.

Thank you 

[johnsonshiue]

Hi Engin,

Many thanks for sharing the files! I took a quick look at the dwg files. I am describing the behaviors without disclosing the files.

I think I know what you are trying to do. You basically want to create drawing views from these dwg files in Inventor, right? There are actually two workflows that you may consider without having to convert the dwg geometry to Inventor sketch.

You can simply link the dwg file to an Inventor part or assembly. You can start a new part -> Import -> pick the dwg file -> pick an origin plane and the origin point to place the dwg geometry. This is called DWG Underlay. Once you bring it to a part, you can create a drawing view in Inventor idw/dwg based on this part. If you want to create solid geometry, you can project the dwg geometry to a sketch.

Another drawing related workflow allows you to use the dwg file as a template. You can simply use the dwg file as a drawing template. Then start a new Inventor drawing from the template.

On top of these workflows, AutoCAD can create associative drawing views from Inventor components. Assuming the AutoCAD release is newer or the same as Inventor, you can use VIEWBASE command in AutoCAD to create drawing views and annotate Inventor components without using Inventor’s drawing environment.

Many thanks!