I'm hoping for a simple fix.
I imported a half completed design(Autocad) into an Inventor assembly file and started to make changes to the part using the hole command and I found that not all of the changes were made to the original part file. Which of course make the creation of detail drawings impossible.
Here is an example:
This plate has six smaller holes and one notch on the side that I added in the assembly file. but when I double clicked (or edited) the part it looks like this:
When I open the part (right click/open) it looks like this:
Notice the center six smaller holes are missing (created with hole command), but the notch (created with sketch/extrude command) in updated to the part.
Is there anyway to merge these holes into the part file?
Solved! Go to Solution.
Solved by GSE_Dan_A. Go to Solution.
It looks like you used assembly features to add the six small holes to the assembly. Delete them from the assembly and add them to the part. It shouldn't take long to do that.
First of all, thank you for your quick reply to my request for help.
When you say delete them from your assembly, and add then to the part, do you mean delete them where they appear in the browser and then open the part and add them there? if so there is problems.
Their location are relative to other parts in the assembly and were there because of features around them which won't be in the part file.
Secondly I have other holes (perhaps 50 or more), tapped holes in a plate that were added relative to the screw clearance holes above them.
You could add the holes to your part but leave them underconstrained (i.e. no dimensions or sketch constraints). In your assembly, make the part adaptive and use assembly constraints to mate the holes to the components that drive thier location.
Another technique would be to use derived components to use geometry from one part to create another.
Here are pics:
The tapped holes were added to the plate using the concentric hole placement using the screw clearance holes above.
I was kind of hoping for some kind of reverse update command.
You can add them to the part while still in the assembly. Fi=rst delete the holes from the top level of the assembly. Double click on the part to activate it, then add the holes. You should still be able to use other features in the assembly as references. Especially if you add the holes by first creating a sketch with points to be used as centers. In your sketch you can locate the points using reference geometry form the assembly.
Hope this helps.
Chris Benner
Inventor Tube & Pipe, Vault Professional
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"You could add the holes to your part but leave them underconstrained (i.e. no dimensions or sketch constraints). In your assembly, make the part adaptive and use assembly constraints to mate the holes to the components that drive thier location."
This sounds doable. I will give it a try. Not sure if I understand this part: "use assembly constraints to mate the holes to the components that drive thier location."
Thanks also Chris B.
I decided to try Chris' solution first. It sounded a lot like what I tried to do at first but failed.
"You can add them to the part while still in the assembly. Fi=rst delete the holes from the top level of the assembly. Double click on the part to activate it, then add the holes."
Ok, I deleted holes and double-clicked on part. the part on top faded and I entered the hole command.
"You should still be able to use other features in the assembly as references."
I tried concentric and On point, but the hole command fail to pick features off of the faded parts. On to the next step:
"Especially if you add the holes by first creating a sketch with points to be used as centers. In your sketch you can locate the points using reference geometry form the assembly"
I created a sketch using the plane of the target part, but my sketch failed to locate or constrain to any referenc parts of the assembly.
Edit the part in the context of the assembly, then edit the sketch for the holes. Project geometry from other components in the assembly for locate your holes.
There is a Add On in Autodesk Labs that will push the features you made in the Assembly level to the Part Level. So any holes or extrusions that you have made at the Assembly Level will be transferred into the Parts.
The Add-On is called Feature Migrator. It works really well!
Information - http://cadsetterout.com/resources/feature-migrator-for-inventor/
Download - http://labs.autodesk.com/utilities/featuremanager
In your sketch did you use "Include Geometry"?
Have you had much Inventor training or experience? This is a great place to go for a start on that: http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
Well the add-on worked and updated the parts to the assembly. 91 holes were transfered to various parts and it took about a half hour (my lunch).
I am a 20plus year Autocad user and a 1 month Inventor user. I completed a 4 day Inventor Essentials class, but bare essentials would have been more descriptive.
I thank you, Chris and Jeff for helping out this Newbie, and I will for future projects ultilize Inventor procedures.
Dan A. Thanks so much for the life saving advice. you saved me hours of redo.
Solved!
Any time! Glad I could be of assistance. I know that feature can be pretty useful (more so if it could handle other feature migrations like chamfers, fillets, etc...)