IAM file & Part Creation

[Anonymous]

Because parts are created in IAM file, there is no constraint on created parts, therefore if I closed and reopen the IAM file, created parts are not there. Is it necessary to constrain created parts or is there any other way to bring created parts back to IAM?   

[Mark.Lancaster · Accepted solution]

@Anonymous

So it sounds like you created a part in an assembly then close the assembly without saving, is that correct?  If so you never wrote the reference to the part in the assembly so when you reopen it, it doesn't know that it needs it.  Meaning just becuase you created the part in the assembly doesn't mean its automatically save in the assembly. 

[mdavis22569 · Accepted solution]

it should be there.  You need to save ..and at the bottom of the save, the new part will be listed and next to it say: Initial Save

https://www.youtube.com/watch?v=AXRjEWDAvWA

you can constrain it in the Iam, you might already have 1 constraint depending on how you set it up.. 

[blair · Accepted solution]

To add to Mark's post, the only way they would not have Constraints is if they were created as Adaptive using projected geometry from other parts in the IAM file. You should be getting some sort of message that not all the parts have been "Saved" in your IAM file when you close the file.

I tend to clear Adaptivity on my parts as soon as I can because of the problems that can creep into a IAM file with too many parts being Adaptive.

You can also make have IAM's that have been created from a Multi-Body part that has the parts pushed out into a IAM file. Generally it's easy to tell because all the parts in the IAM file are Grounded.

[Curtis_Waguespack · Accepted solution]

Hi fiatnm,

Yesterday we discussed the adaptive settings, and why we might turn those off.

As mentioned this is my preferred method, as it does not create adaptivity unless I choose to (by using the CTRL key when project geometry), but it does require us to constrain the parts, where as using adaptivity would not require constraints.

So if you are watching Youtube videos and have the adaptive options turned off, it's likely you will need to do some extra constraining that the video authors do not do.

I think the others are correct in that your assembly didn't get saved and that's why the part was missing, but the constraints might be due to the settings, if you turned them off.

Here are two quick videos.

In the first I leave the option in the Create New Part dialog box on, so one constraint (a Flush) is created automatically. Notice that my new part is not adaptive, and not constrained in place, so I add an insert constraint. The Flush constraint becomes extra, and could delete if I wanted.

In this second video I remove the option to create the Flush constraint automatically as I create the part. I still add the Insert constraint though. 

I would need to save the assembly at the end of these videos, in order for the new part files to be created on my computer (it only exists in Inventor's memory, until I save it), and I need to save the assembly in order for the assembly file to record the link to the new file also.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Removing the check mark, placing two locks. I am not clear about this.

[Curtis_Waguespack · Accepted solution]

Hi fiatnm,

You are correct. Rather than making the sketch geometry adaptive to the other part, when we clear those options, it makes the circle the same size and location as the other part and applies Fix constraints to lock the sketch geometry size in place. You can delete these constraints and apply your own dimensions and constraints if it helps you.

But whether we use adaptive geometry or fixed geometry, when we project from one part to the other we should take the time to ensure that the sketch is properly constrained.

Another approach is just not to use projected geometry, and simply sketch the circle as we would if creating the part by itself, and then apply dimensions and constraints like we would normally do. 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Thanks