Work planes and sketches keep reappearing??

[Anonymous]

This isn't down to just one model, but work planes and sketches keep reappearing on models within assemblies.

The most recent has models that have hundreds of work planes, and each one has reappeared. If I open the model, there are no planes.

How can I stop this from happening? It's going to take hours to change the visability. I know I can change it via 'Object visability', but that really isn't solving the problem.

Any ideas?

Thanks

[Anonymous]

Thanks again Cris,

Following your example I was able to hunt down the content center part and link the NLG parameter into my assembly and assign it to my LENGTH in the assy. Once I went to my CC bolt part and did a change length, it lost the link and shows the old value. ("L_OLD in the attached pic is still being driven by the sketch and shows the new length.)

It is very common for a fastener to change length, and the sketch with reference dim follows that change.

It also was very hard to hunt down the correct fastener out of the content center folder.

I think we can live with the sketch thing - your tip of 'select all occurences' will be a huge timesaver for resetting DVR back to Default.

I think the right solution is for IV to maintain DVR when you turn visibility for subassy's on and off, as you suggested.

Hopefully that happens.

Cheers,

Ben

[Anonymous]

Hi,

When you changed length of the bolt I assume you have replaced bolt with another one from CC.

Linking parameters is not relative to your assembly but uses full paths and has no association with components in assembly.

If you changed bolt to create another fastener assembly of yours, and left old one unchanged it would still work if you relink your parameter to bolt currently in assembly.

If from the other hand you often need to change bolts in a single assembly (witch I hardly expect to be the case, because in such solution this would change everywhere this assembly was used) this will not work efficiently for you.

I thing that in the long term it would be more convenient and less time consuming to have assemblies linked to a given bolt as long as you would not want to change this bolts in a given assembly often.

Cris.

[Anonymous]

Operation: toggle on and off visibility

Normally one would think it is as simple as right clicking and turn off the visibility, perform task(s) while part is invisible, then turn the visibility back on.  The problem is, like already stated, the planes turn on with it.  The fix is, instead of right clicking and turning visibility on select Representation instead.  Then select default as the design view representation.  As long as you have your planes turned off in that assembly or part in the default view the part turns back on without planes. 

[amichaudJ6E3R]

I have a similar issue in my assembly,

my view rep is set to Default, however, when I toggle the visibility of my part on and off, the work features and some sketches keep reappearing regardless of being turned off IN the part?

I don't get it...I must be missing something somewhere?

I'm on Inventor 2020

[johnsonshiue]

Hi! I don't think you miss anything. When you said you activate "Default" Design View Rep, I assumed you were talking about the top-level assembly. Based on the behaviors you are describing, I think the visibility change you made was one of the two cases below.

1) You turn off workplane/sketch visibility within the subcomponent files (not edit-in-place; open in its own window). But, the Design View Reps are not linked to the top-level assembly.

2) You turn off workplane/sketch visibility by editing subcomponents in place or from top-level assembly. The change is only stored within the top-level assembly. The workplane/sketch visibility is still on within the subcomponent files.

Right-click on the part or subassembly which you see visible workplane/sketch -> Representation -> Design View. Is it set to Master or a non-Master DVR? If it is Master, it means you did one of the two workflows above.

The correct way to make sure visibility is consistent across multiple assemblies is to link Design View Rep. Go to Representation -> Design View -> change it to a primary non-Master Design View (Default). Open the subcomponent in its own window. and turn off visibility there -> Save. Now, all assembly with a link to this subassembly Design View Rep will inherit the same behavior (invisible).

Another place to change is the File Open Options (Tools -> App Options -> File). Make sure Default is selected in Design View Rep for Assembly and Part.

Many thanks!

[amichaudJ6E3R]

Hi,

Thank you for replying so fast. I've tried everything you mentioned, nothing worked. Unfortunately I can't share my assembly but I'll try to describe it as best as I can.

My top level VR is set to Default (not master).

I did like you said, right-click on my part/representation, and changed it from Master to View1. Went into my part file (separate window), made sure everything was turned off, then saved.

Now everything is invisible, but if I hide my part, and unhide it, everything reappears and the view rep (of my part, in my top-level assembly) is reset to master

I went into the App Options/App settings, and made sure that it was set to non-master VR. Even then, if I hide/unhide my part, the work features/sketches reappear...

[johnsonshiue]

Hi! I am sorry I think I misunderstood the issue. Indeed, by making the part invisible and visible, the linked DVR is broken. I think the correct workflow for you is to open the part in its own window -> activate DVR: Master -> hide the workplanes. Then the workplanes will not be visible after you make the part visible at the top-level assembly.

Many thanks!

[danielGW92Q]

it helps!!!