Is it possible to manage a second part state

[Pjone kenobi]

Hi,
I try to manage a second state in my part:
My first state is an inflated state and it is used in my assembly.
Now, I want to manage a "cold" state (non inflated) to realise a drawing part.
I want to keep the assciative link between both.
is it possible to do this? If yes, how to do?

Kind regard
PJ

 

[Pjone kenobi]

Hi,
No Idea?

Kind regards
PJ

 

[Toost]

the description you have posted so far is a little vague for us/me to propose a method,
as of now, i have no clue on what it is that is inflated,
or how the shape changes when inflating,
- can the deformation tools in NX handle the case or not?
the material, does it bend like a cardboard box or does it stretch like a rubber balloon ?

Regards,
Tomas

 

[NutAce]

There a few options for this.

You can create 1 part and have 2 different reference sets where you create a separate body for each state. (1 state in 1 reference set) (not the preferred way of working)

You can create 1 part which is deformable. The deformable result will be the state you use in your assembly

You can create 1 part showing the cold state and then create an additional "Altrep" part showing the assembled state. This part can be used in you assembly.
Because I have never worked in a production environment outside TeamCenter I cannot without a doubt say that this solution is available working only Native.

There might be other ideas / solutions floating around on the web...

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Pjone kenobi]

Dear All,

First, thanks for your help and your reply!
Second,
@Toost: imagine you use an homotetic function: 1 set is the normal part, the second is with the homotetic transformation. But the part is the same.
In my assembly, I used the homotetic version and on my drafting part, the normal part. An idea for how to do?

@NutAce:
sol_1: if I understand well 1 body for 1 state? but is the bodies are with associative link?
sol_2: could you explain me very quikly, how to do? ;-)
sol_3: sorry but I don't understand what you mean by "Altrep"

Kind regards
PJ

 

[NutAce]

Hi,

Sol_1;
You are correct. One body for one state. And if they can be linked with an associative copy is depending on how much they change form.
Difficult to say without knowing how they both shall look.

Sol_2;
A deformable part gives you the option to change the values (in context of an assembly) of the expressions which are driving your body. It cannot be quickly explained.
A deformable part can be used multiple times in the same assembly, where each instance of it can be shown in a different state.
Take a look at below video on YouTube..It will give you an idea what you can do with this.
Deformable Part in NX

sol_3;
Altrep is short for "Alternative Representation". With this you create in Teamcenter a second NX part for the same item. This Altrep can then be used in an assembly to show the same part, but in a different form.
Drawback of this solution is (compared to the deformable part) that you can show only 1 alternative state per Altrep.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Pjone kenobi]

Dear NutAce,

Thank you so much for these clearly explanations!
For the moment, we couldn't use the sol_3 because no TEAMCENTER...
I will watch the YOU tube file to learn how to do a deformable part.
We already used the sol_1, but it's not perfect!

I will keep you informed.
Thanks a lot for all.

Best Regards
PJ

 

[Pjone kenobi]

Dear NutAce,

I've tested the deformable part but my problem is:
If I forgot a hole in my part (for example), I can't add it. I mhave to destroy my deformable part and create again right?

Thanks for your confirmation or not

B/R
PJ

 

[jerry1423]

You do not have to destroy your current model.
What you need to do is to put the hole in the model before the DEFORM (I am not sure of the specific name) in the model tree.
So, look at your model tree in timestamp order and make the feature before the deform the current feature (RMC on feature, make current feature).
Next, Add the hole to the model.
Now make the last feature in your model tree the current feature.
I hope it worked for you.


Jerry J.
UGV5-NX11

 

[Pjone kenobi]

Dear Jerry,

Maybe I made a mistake when I used the deformable part function because when i tried to add one hole BEFORE my deformed state, I had a dialog box which explained me that it was impossible to modify the current model if I already create a derfomable part.
For the moment i can't try again because we follow another solution but I will try again soon and make you a feed back before the end of the week.
Thanks for your help.

Best regards
PJ

 

[NutAce]

You do not have to destroy your current model.

Not completely true. It depends if you want to make the hole Deformable as well.
If that is the case, you will have to delete and recreate the Deformable feature.
Siemens has not yet developed the Deformable Feature in such a way that it can be edited (I am waiting for this for at least 10 years already)
Would also be nice if it can reference Expressions with associativity as well....

If the hole is not needed as part of the deformation then you can do it like Jerry has described.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Pjone kenobi]

Dear NutAce,

Thanks for your lightning on the deformable part subject.
I need to perform on this subject... ;-)
My hole have to be deformable so If I understand well I only can destroy the deformable feature.

Thanks for your help.

Best regards
PJ