Autodesk Inventor

[#1]

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?

[#2]

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.

[#3]

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.

[#4]

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.

[#5]

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.

[#6]

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.

[#7]

"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.

[#8]

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.

[#9]

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.

[#10 · Accepted solution]

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