override position and deformable part in one reusable assembly 1

[Lars1978]

Hi All,

I have a question. I'm engineering a conveyor with supports to the ground. This support consist of various parts (aka an assembly).
The conveyor is not horizontal so each support has to have it's own length. (see attachment)

Except for the variation in length the support is the same. I'm thinking about using override position for the connecting lips and make a deformable part for the part witch changes length.

Does anybody have a good example ?

Kind Regards,

Lars


Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[Ehaviv]

How many supports you have
I mean how many variations
I their are a few say 3 5 variations
I will make 3 5 supports subassemblies
It's easy after making one do save as
And make the variations [ul]
[li][/li]
[/ul]

 

[SDETERS]

We did something close to this for our assembly lines. We used the reuse library and made these "legs" into many different solid bodies in one component and put this in the assembly as one big component vs many components. I was going down the override position and deformable part route also but this does not work well with making a "cut list" or parts lists..

 

[Lars1978]

To a984928

unlimited variations because we use this support a lot. I like to add the support and then constrain the bottom of the leg to the floor the top of the leg to the conveyor.

SDETERS
Ok you say when making a bunch of solid bodies in one component with the reuse library. Does anybody know how if the deformable part thing works ?

Kind regards,

Lars



Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[Ehaviv]

Yes deformable part thing works

in menu tools choose define deformable part
then choose the part to be deformed
and then choose the length expression to be changed when you bring the part to the assembly
and go thru all the pages and finish

Then when you add the part to the assembly and after mating the part in place
you get a dialog with the length expression set it as you want

and you can use repeat to facilatate the work

Works but not easy if you have many supports

 

[Ehaviv]

Open the part to be deformed and then choose tools ==>> define deformable part
and continue as abouve

 

[Lars1978]

can it be done when you have one subassembly support with deformable legs. I mean can I insert this subassembly many times and then change the lengte of each leg (in each subassembly) individually ?



Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[Ehaviv]

I think no because the define deformable part works only
on part features such as extrudes sketches or any object on the part navigator

You can try to mix in the subassembly part navigator features that afect the change the lengte

So your subassembly cosist of features and components

 

[Ehaviv]

Sory the above is thru but not for your question

I tried what you mean and that not works because all subassemblies will be deformed the same

So you can try the mix as in the previuos post or build the subassembly as one part

 

[Lars1978]

Sdeters can you give a example or a way to go when making this reuse library solution ?




Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[SDETERS]

Have a look at the PRT file I have attached. Kind of hard to explain on how we did this. please Go into the expressions. I have some setup for the length and other parameters for this weldment. I have stripped some stuff out of it, so all of the named expressions may not work well. But you should get the idea.

We use teamcenter. Our goal was not to have million different part numbers, for each different length of extrusion or shape, in all of our assemblies. We originally went with deformable parts but it just did not work for us. We call this technique using a weldment.


So we modeled our shape with the coordinate systems at the ends to control the lengths, and which in turn modifies the attributes in the "solid body" to our cut lists.

What We did is use reusable object command with the "body" option toggled on in NX to define this reusable object we modeled above.

We set up expressions with sketches, coordinate systems, or what have you in a new part. We drag and drop these reusable parts into the model from the reusable library into this new part. Then we use the three coordinate systems that are in the usable part, to place the reusable part into our model. In the History tree they are named Base (Which defines start point) Base end angle (controls if you want to miter the start end) End length and Angle. (Controls the length and angle of the end of the shape.)

We also set it up with the coordinate systems to define the cut lengths in the solid body attributes. Imagine the coordinate systems with the solid body being put onto a miter saw and cut. So we have angles, lengths in the solid body attributes which automatically will spit into a special cut list. There is a special way of getting this into your 2D drawing parts list. I can supply the drawing if you would like this also.

Kind of hard to explain, but hopefully this gives you an idea of how we accomplished this. Maybe there are some other or easier ways of doing this. Once you set this up and you have Product Template studio, you can modify this through Product template studio instead of through expressions.

Also once you get a model set up, it is really easy to modify an existing one to get a new weldment

 

[Lars1978]

SDETERS,

Thank you for the quick reply. I've seen the file. What I see is a part file, not an assembly.

The thing you mention above is this strictly for a part file or can it also be an assembly with the 'leg' parts changing in length ?

Kind regards,

Lars


Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[SDETERS]

Correct it is a part file not an assembly. The leg parts can be the reusable part that change in length and added to your assembly as a component. So your part file will have 100 legs with many different lengths. This solution may not be what you are after.

You can also have different components in this file also. But the point of doing this is having different length extrusions, steel shapes as solid bodies not components.

So our assembly looks like this.

Assembly Station Main Assembly (Torque tools, Electric Boxes and Weldment sub assembly)

Weldment subassembly (with mounting plates, screws, "different length weldment")​