Inventor 2019: Import AutoCAD geometry into Inventor

[lkirit2000]

Hi 

I have a roof profile  (section ) in Autocad file. How I can import into Inventor  2019 part file to create a 3D model ?

I have attached AutoCAd file.

Rgds

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@lkirit2000,

marius.gildehaus has edited your subject line for clarity
Original: Import AutoCAd Drawing

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[marius.gildehaus]

Hello @lkirit2000!

I made you a short video here:

 Also in attach the dataset.

Thanks!

[johnsonshiue]

Hi! Marius shows one of the ways to do that. There are other ways too. You can also link a dwg file to an Inventor part. Start a new part in Inventor -> Import -> pick the dwg file -> pick an origin plane and the origin -> the profile will be inserted to Inventor as underlay. Then you can create a sketch on the same plane or any plane and use Project DWG Geometry command to project what you need from the underlay. When there is change in the dwg file, Inventor will be notified and you can update it associatively accordingly.

Many thanks!

[lkirit2000]

Hi,

That both methods are work well. Thanks !

I am trying to make a sheet as shown in the attachment, but when I couldn't select the whole sketch as once.

Please let me know how to do that ?

Rgds

kelly.young has embedded your image for clarity.

[johnsonshiue · Accepted solution]

Hi! I guess there are gaps between the lines and curves in the AutoCAD dwg file. If you copy and paste the lines from AutoCAD to Inventor, you can use Sketch Doctor to help close the gaps. Here is what you need to do.

1) Finish sketch.

2) Right-click on the sketch in the browser -> Sketch Doctor -> click Next all the way. You may be prompted to select the points to create coincident constraints.

If you cannot figure out, please feel free to attach the Inventor file here. Forum experts can help take a look.

Many thanks!

[lkirit2000]

Hi 

I did the sketch in both ways ( copy - paste and import )

I have issue with the both ways in the extrusion.

I couldn't find sketch doctor when I right click in the sketch ?

I attach the both for you to try and let me know ?

Rgds

[johnsonshiue]

Hi! Sorry, I forgot about the dwg file you attached. I will take a look first thing in the morning tomorrow.

Many thanks!

[kelly.young]

Hello @lkirit2000 if you RMB on a line within the 2D Sketch and select Close Loop you should be able to select the line for Extrude Surface all at once.

Please select the Accept Solution button if a post solves your issue or answers your question.

[johnsonshiue · Accepted solution]

Hi Kiri,

Sorry to reply to you late! Day job is taking away my attention here. I took a look the dwg file. There are problems in curves. First, there are big gaps. When you try to extrude it as a surface, you can only select the left portion. If you zoom in closer, you will see there is a gap about 0.002in. This is too big. Inventor 2D sketch is precise up to 10E-9mm.

Second there are overlapped curves, particularly in the middle "hump." The arcs at the top and the adjacent curves are all overlapped. This can cause profiling issues. You need to clean up the geometry either in AutoCAD or in Inventor. The sketch in such conditions are not ready to be consumed by a feature.

Please keep in mind the geometry you create in Inventor cannot just look about right. It has to be precise. The tidiness will help you build a robust model, easy to edit. It may seem restrictive at first but you will find it a good habit to keep. Building high precision model needs some disciplines.

Many thanks!

[WHolzwarth]

I've tried for an acceptable result with Inventor, too. I could import the dwg, and deleted the outside lines of  the central sketch, that could be patternd. But I had no luck with a surface extrusion.

Sketch Doctor showed lots of disconnected points, but was not able to join or clean-up the sketch.

Therefore I opened the DWG in Rhino 6; extrusion was no problem there. But it showed lots of duplicate faces.

Nevertheless I opened the result back in Inventor (see 2018 IPT in Zip). Now it's obvious. All faces looking in darker yellow are duplicate and need to be deleted. After that joining to a single surface will be possible.

I'll try it later and will come back, if there are further problems

[WHolzwarth · Accepted solution]

Result in attachment, placed vs origin planes and ready for mirroring and pattern operations.

2018 IPT and STEP in Zip

[TheCADWhisperer]

What is the source of your AutoCAD dwg geometry?

I can create a step-by-step analysis video of the issues with the geometry if interested.

[lkirit2000]

Hi Team,

I have imported the sketch into inventor part file. 

Now I need to do Surface extrusion. But I couldn't select the all line at once. 

Also sketch doctor also not working ? 

Please guide me the correct way !

I have attached the file.

Rgds

Rgds

Kiri

[WHolzwarth · Accepted solution]

You've imported as DWG Underlay. Now you can follow the steps in this description:

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2018...

2019 IPT for starting is attached. A small gap needed to be closed manually (hiden in Stitch feature)