Weldment Question 2

[behindpropellers]

I am a bit unsure on how to use the weldment feature in SWX. I can design the parts in the weldment profile, but how do I get the parts out that are machined?

I am mainly looking for advice on how to extract my parts out of the weldment so that we can have them CNC cut.

This is my first time using the weldment area of the software so any tips would be appreciated.

Thanks

 

[davidinindy]

It's hard to understand exactly what you're trying to do.
You need to create the machined parts as regular solid parts, then add them to an assembly with your weldments.
It sounds like you may have created a multibody part?


David

 

[tbryant]

Use the Split Part command to save the bodies out as individual part files.

 

[CorBlimeyLimey]

Check out Weldments & Relative View from the SW Help files.

A weldment creates a collection of bodies (each structural member is a separate body} within a single part.
If a member needs to be machined, the details can be shown using the Relative View function. This creates a separate view of the member.

NOTE: The above is for SW04. I'm not sure if 05 & 06 has changed this.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[behindpropellers]

I eventually found out what I had to do.

I had created a weldment and then modified the parts within the weldment. I was stuck at the point from when I wanted to take the parts out of the weldment.

If anybody else needs this:

1. Right click on the member you want to export.
2. Insert into new part.

Thanks for the helpful replys.

T

 

[CorBlimeyLimey]

behindpropellers ... Be aware that by doing what you did, the part is NOT associative with the weldment! If you change the weldment, the "Inserted-into-new-part" will not change.

If you use the Relative view method, it will remain associative to the weldment.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[behindpropellers]

Thanks for the heads up. I will look further into the relative view method and go from there.

T

 

[J-C]

Insert into a new part will remain associative, just more files to deal with though.

Jason

 

[CorBlimeyLimey]

I stand corrected. Thanks Jason.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[alolesen]

I use the “relative view” technique quite often. It allows you to pluck a single body from a multi-body part file, like a weldment, and drop it onto a drawing sheet all by itself. You may then pull views off it, section it, what ever you like. The only thing to remember is that you need a pair of flat faces, at right angles to each other, in order to define the relative view. In the case of cylindrical bodies you may need to include a tiny flat surface on the side of the cylinder for this purpose. All of the associativity, to the weldment, is maintained.

 

[behindpropellers]

Is there any way to have a linked property that will pull the split part names into a drawing of the original weldment?

Thanks

 

[Knotfreak]

How can I proceed if a seperate machined part is welded to the weldment structure?

Take a dune buggy chassis for example.

My guess is that modeling a dune buggy chassis using weldments is not the best approach.

 

[MMike1]

FWIW, we do nothing but steel structures where I work. Flat bar, HSS, angle, channel etc.... I gave up on using weldments. It just doesn't do what I want. We drill, mill and punch holes in stuff before it gets welded. It's just easier to creat an assembly.

I got all excited at the prospect of using weldments when we switched over to SWx, but it just wasn't to be....

 

[CorBlimeyLimey]

I have not used Weldments in a "real world" environment, just online tutorials & practice, but ...

Knotfreak ... If you cannot add "standard" machined parts directly into a weldment, that would make for a good ER. Till then, could you not add the Weldment into an assy & then add the separate machined part.

MMike1 ... I'm suprised you find assys easier. Using the assy method you have to add mates & end up with multiple parts to keep track of.
Using the Weldment method the layout sketches take care of the mates. It is also very easy to "drill, mill and punch holes" in the weldment bodies and produce separate machining drawing views of each body without ending up with multiple parts.
Obviously everyone has their own preferences, but I'm just curious inquisitive (OK, OK ... nosey), what do you want Weldments to do?
Maybe the improved 3D sketching in SW06 will make Weldments easier?


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[coolcad]

Maybe I'm missing something, but we do this all the time. We create fabrications (weldments) and then machine them to a finished part. The first thing you do when creating a weldment is to hit the "Weldment" icon to establish this part as a weldment. Then model your part as it is welded together. Then add all the machined features. Now flip to your Configurations tab and you will see two configs, <As Machined> and <As Welded>. Switch to the <as Welded> config and go to your model tree and suppress all the machined features. Then we create a drawing of the part in the welded state using the <as welded> config and a drawing of the machined part using the <as machined> config. Our NC guys then use the <as machined> config for their programming.

If we have items in the weldment that need to be cut on the torch table or waterjet then we go to the <as welded> config and do a "relative" view of that item. Then they can use that view to create a dxf to export to the burning table.

I hope this is what you are looking for.