Autodesk Inventor

[#1]

Is it possible to make visible or part that is suppressed?

My situation is that I'm creating a generic drawing that will show multiple configurations of one of our products.  We have optional output customer connection styles.  I showed the most popular style but I need to show one small part for the inspectors to know that it sometimes may be there.

The issue is that this is in a detail view of the base view and I can't change the base view, I need this to only effect the detail view.

Any advice would be greatly appreciated.

[#2]

If you use Design Views rather than LOD you will be able to get what you need. You should not be using LOD to turn items on and off in a drawing.

http://forums.autodesk.com/t5/Autodesk-Inventor/What-does-this-Assembly-Message-Mean/td-p/3344085

Post 8 onwards may help.

Regards

Martin

[#3]

There was a reason that I chose LoD over Design Views.  One was because my system is/was 32bit running XP.  Another reason had to do with using certain LoD's within other assemblies.

I'm going to look into Design Views though.  Thanks.  Not sure it will help me right now though.

[#4]

Maybe I'm missing something here, but could you not have this optional part turned on in the LOD, then turn its visibility off manually in the views where you don't want it?

To turn it off manually, just find the part in the browser (under the appropriate view), right click on it, and uncheck Visibility.  Note that if this doesn't work (Visibiilty is grayed out), it typically means the view is set to be associative to a view rep.

An alternative to this manual method would be to use your LOD as-is, but then also have view reps with and without the optional part.  You can set both an LOD and a View Rep in a drawing view, so the options don't have to be mutually exclusive.

[#5]

The *.iam file is setup so that each LoD is a different possible customer configuration.  It's a tank weldment where the main body of the tank and the input junction box are the same on all configurations.  The output is what changes depending on customer need.  I setup LoD's for each tank output style in the tank weldment *.iam.

Then in the overall assembly I created a LoD for each different style of output configuration.  I also created a few LoD's for detail views of certain parts or areas of the assembly that i needed to show.

The issue I'm having is that I need to show in a detail view one part (a compression lug) as an optional part.

As of right now I just editted a balloon and force it to the right item number on the list and pointed to the area where this part would be located.  But depending on the inspector they may want to actually see it on the drawing (which they probably will considering the multi-page list they sent for us to follow for certification).

[#6]

That would seem to lend itself to my LOD / View Rep combo idea.  I think you could do the following:

1)  Have the lug active in all LOD's.

2)  Turn visibility off for the lug in the Default View Rep

3)  Create a second View Rep with the lug visibility on (ex.  Lug On).

4)  For all your "main" views, use the appropriate LOD and the Default View Rep.

5)  For your detail views, use the appropriate LOD and the "Lug On" View Rep.