Doe it mean that the master view rep is automatically always locked?
I'm super ultra frustrated with this. I have models with a many planes and sketches in it. They're all fine, it just crowds the screen when they're all on. Here's where I pull my hair out:
I get the part model looking just how I want. I mean, instead of using the master view, I make my own called default. Boy it would be super fantastic if I could just set an option to use the default view when the parts are inserted into an assembly instead of Inventor requiring me to use the master view. Ok, but for now, I have to insert the part, right click on representation, and choose default view. So, it’s just a minor inconvenience. No hair pulled out yet. Here’s what burns me up. When I uncheck the visibility box, the part is no longer visible. So far, so good. When I check the box to make it visible again, what do you know, it’s switched over to super horrible looking master view. I never asked Inventor to switch views, but it went ahead and did it anyway. So, now I have to right click, representation, default view etc. Still not pulling my hair out, but thinking about it. Ok ok ok, I have it figured out. I’ll make the representation associative right? Then when I turn my model back to visible, it should update the view to wherever I left the default view in my model right? Fantasic. But, it doesn’t work. When I uncheck the visibility box, I get an error message requiring me to remove the associativity. First of all, why do I get any kind of error message just for unchecking a visibility box, com’on guys… Second, why can’t the part be unvisible and become visible again with the same representation? That’s when I pull out hair by the fist full. Why MUST I have to go through the master view? It might not be that bad if I could CHANGE THE MASTER VIEW, but I can’t. Inventor is forcing me to use the master view and won’t let me change it. Very, very frustrating.
Hi jaxonusa,
As a rule of thumb it is best to always right-click on work features and sketches in the part file and turn off the visibility there. This prevents the issues you're having with the visibility of these things turning on and off at the assembly levels.
You can then control the visibility of the work features and sketches in the parts at the assembly level as needed.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Well, that's what I'm doing. I can get the view in the part file to look the way I want it, but not in the part file master view. The master view is the one what gets used when the part inserted or checked back into visibility, and that's the one that can't be changed.
The only thing that I can think of to toggle the visibility of parts while keeping workfteaures invisible at the end of the ride is to LOCK the viewrep:
1) Lock the active viewrep (ie. View1) in your assembly
2) Turn off the visibility of one or more parts
3) Do whatever you need to do ....
4) Activate the Master view rep of your assembly
5) Activate View1
6) Unlock View1
This will bring you back to the initial situation with the parts visible without seeing unwanted workfeatures and withour the need to activate viewreps in any of the parts.
Bob
I have this issue too, also with Enable/Disable. Locking a view representation removes the associative representation links, so it is not without side effects.
Also when adding a new component to the assembly I have to remember to link all the representations as desired. I'm thinking of automating the associations as my views usually follow a pattern (Assembly -> Component): Default -> Default, Design -> Reference, Reference -> Default.
I wish the visibility of origin features was remembered by the view representations. Also that view representations were applied to iPart members based on the iPart factory, or there was some way of applying visibility/enabled to the derived features.
Just ran into this same issue today, several years later. Using inventor 2016. Still have one or two strands of hair left......
I too have had this issue. The concept of design views sounds good, but I have yet to see an implementation that doesn't require us to hire people with no hair...
Hi Steven,
This is a very old thread. Some of the comments may not apply to more recent releases. Design View Representation can be applied to an assembly or a part. It depends on what you want to achieve, there are workflows to help you accomplish your goal. I don't want to get into detail yet because it can overwhelm you. Could you tell me what exactly you want to do? I should be able to tell you the best workflow to do that.
Many thanks!
I think it is worth pointing out that the padlock symbol means different things depending on whether you are in a part or an assembly.
I may be simplifying a bit here but...
In the part file it locks out only section view (use other view reps sparingly for sections if you don't want view rep lock errors on save)
In the assembly file it locks out section, visibility, appearance overrides
Therefore in a part file you should turn off work features in master view. Place the part into an assembly so that the default and other views display the part master view - no change of view rep necessary.
It is a conceptual mess but works 98% of the time.
Hi! Just put a little bit historical perspective here. Indeed, the Master Design View in Assembly has a different behavior in Part. DV:Master in Assembly was implemented more than 15 years ago. It allows users to configure component appearance in a given assembly along with work geometry visibility. There was no Part Design View until 2012. Part Design View generally works fairly similar to Assembly Design View. But, there are major differences.
First, DV:Master in Part is basically as is. Overrides can be saved in Part DV:Master, which is not allowed in Assembly DV:Master. The reason why it is designed this way is to support the legacy files already contain part level and body level color overrides. If Part DV:Master strips off the existing overrides, the files will have to be migrated and a new DV will have to be created on open. As a result, the behaviors are different.
Second, Part DV has to interact with feature history. For example, you can move EOP or edit a body generating feature, the body will not exist and the body color will be put on-hold. Work geometry and sketch would have similar behavior. Assembly DV pn the other hand only needs to care about individual component occurrence. There is no history tree in assembly except assembly features. However, Assembly DV does not control assembly feature appearance anyway.
Anyway, this is a design choice made by the Inventor team. There are certainly pros and cons. So do other proposals.
Many thanks!
Hi, I have a skeleton model that I use for our design process. It uses work features to place and size components in our assemblies and parts. However, because of the large number of parts that we need it is difficult to manage.
I was trying to use the design views to change the "mode" of our skeleton. Modes could be Part Design, Component Placement, etc. Each mode shows different work geometry and features that the end user will leverage while creating parts. Unfortunately, I wasn't able to wrap my head around the design view concepts.
Thanks to @50h9j for explaining that assembly and part design views are intended to operate differently. At the end of the day, I am trying to setup design views, but when i have to change/ add components, where should I be working? In the Master Design View? If so, I then have to go through each other design view and hide all the new features. Just seems like a lot of extra time.
If anyone wants to pm me for more info, I can provide some models.
I know this is a slightly older thread, but I have been having a similar issue. The view representations are all well and good, but what I don't like is Inventor changing the view representation of my assemblies back to locked Master every time I go to save. I have NO idea what is causing it to switch back and it's really annoying. Looking for any insight because I've looked in Options if there is a setting that tells it to switch to Master, but haven't found anything.
@karipates6709 wrote:
I know this is a slightly older thread, but I have been having a similar issue. The view representations are all well and good, but what I don't like is Inventor changing the view representation of my assemblies back to locked Master every time I go to save. I have NO idea what is causing it to switch back and it's really annoying. Looking for any insight because I've looked in Options if there is a setting that tells it to switch to Master, but haven't found anything.
@karipates6709 Often that is due to suppressing parts or similar..
Are you trying to suppress parts in view reps?
No. I may turn things off or on visibly, but avoid suppressing so I'm not changing the level of detail. I've only noticed this start happening in the last couple weeks. Visibility of parts shouldn't change the view representation. When I see the error about saving with it in a locked view representation then I switch it to the unlocked Default, but it doesn't stick for some reason.
@karipates6709 wrote:
No. I may turn things off or on visibly, but avoid suppressing so I'm not changing the level of detail. I've only noticed this start happening in the last couple weeks. Visibility of parts shouldn't change the view representation. When I see the error about saving with it in a locked view representation then I switch it to the unlocked Default, but it doesn't stick for some reason.
@karipates6709 Do you have an assembly in which this issue is repeatable/reproducible to share with Autodesk?