Hello- Someone has given me a .wire file from Alias. I fired up a new assembly in Inventor but it imported into a part. There are many parts to this design, and I'd rather have them as separate parts. However what I have now is one part with many surfaces (which I can turn on or off). Does anyone have any tips for bringing it in differently? Maybe I can derive some parts out from my existing part which has about 20 surfaces (which should be parts)?
Many thanks in advance.
Solved! Go to Solution.
Solved by AustinLiu. Go to Solution.
Hi, dalibu,
In Alias Import Options dialog box, select Non-Associative Import radio box, go to Create Surface As dropdown list and select Individual Surface Bodies.
Regards,
Kevin Li
SQA Engineer, Autodesk, Inc.
Thank you very much for that tip. I found the settings, but it didn't change the fact that the surfaces all ended up in one part. I am using Inventor 2013.
Hi dalibu,
In order to narrow down and make sure I understand your problem precisely, can you list the detail reproduce steps of your problem and expectation here ? It is appreciate if the .wire file can be attached also.
Regards,
Kevin Li
Hi Kevin. Thank you for your offer of help. I will be able to provide the details and a .wire file on Friday. Meanwhile I've been sidetracked onto another job.
Regards,
David
Hi dalibu,
Thanks so much for your support ! Looking forward to it.
Have a good day!
Regards,
Kevin Li
SQA Engineer, Autodesk, Inc.
Hi Kevin,
I couldn't attach the original files as they are confidential. Therefore I made up a quick file in Alias which was very simple as I haven't learned Alias yet. Then I imported it into Inventor. As you can see the blocks came into one part, but I would prefer them to come into an assembly. Attached is the .wire and .ipt as well as screenshots. Hope you can make a suggestion for me. Many thanks in advance,
David
Hi,
Thank you for your feedback.
I am sorry to say there is no way to import the Alias file directly as an assembly in Inventor, because the design in Alias file is actually in one part, no assembly hierarchy.
So we need to work in Inventor to convert them as assembly.
I tried your sample, and here is what I did:
1. File->Open, choose the Alias file
2. Click on the Options dialog, and:
1) Choose: Non-associative Import
2) Check on "Import into Repair Environment"
3) Choose "Create Surface As"=Multiple Composite Features
4) Check on "Auto Stitch"
3. Click OK and Open the file--here we will see that the closed surfaces now are converted to individual solids.
4. Go to Manage Tab, and choose Make Components in Layout group
5. Select all bodies.
6. Click Next Button and then later the OK button
7. Here we get an assembly.
Please be noted that in #3 we should ensure we are using all "closed" surfaces; if some surfaces cannot be converted to solids, we need to work in Inventor to make it solid first.
I attached one document to introduce this workflow for your reference, and please let me know if any further questions.
If something confidential that cannot talk on Forum, feel free to contact me via email directly.
Thanks,
-Austin
Hi Austin,
I'd like to thank you for your detailed reply. I tested importing my blocks.wire file using your Word doc instructions and I was able to make an assembly with separate parts very easily. This is exactly what I needed.
With this technique associativity with the Alias file is not possible, but then it is more convenient to work with separate parts in Inventor.
I think these files could be useful for others on the forum who are looking to import Alias files into Inventor.
Thanks again,
David
Hi David,
Glad to see it works for your on this case.
Feel free to contact me via email if any Data Translation related issues or questions in the future. Any feedback is highly appreciated.
Thanks,
-Austin