I have only been using SW for a while now.
I was hoping some one could please let me now how to split a frame into seperate part files.
Please let me know if you can help.
RMB on a body and choose "Insert into New Part". By the way, if you want to seperate the weldment bodies for detailing then you can use the Select Bodies function (see below) to show and detail individual bodies in a drawing. Then you won't need seperate part files. If you want seperate part files for another reason, then nevermind.
the insert relative view option is nice for breaking weldments for detailing
I'll second what Glenn said. We use the "Insert into New Part" option because we have many of our blanks produced by an outside tube laser cutting vendor. They need individual part files. We also use the same functionality in our multi-body sheet metal parts because we have several of our blanks produced by an outside water jet cutting vendor.
But we use the drawing / select bodies functionality to capture all the individual weld part details in a single drawing so our fabricator doesn't need a stack of separate drawings to put together the weldment.
Depending on your needs, both methods have their place.
If you place a relative view into the drawing, is there a way to have a lable linked to the item number?
We typically add a model view and then use the "select bodies" option in the property manager to isolate individual weldment bodies. The balloon functionality works just as expected pulling item numbers from the weldment cut list.
But just to check, I opened an existing drawing, created a relative view and set it up for a single weldment body, and then added a balloon to the view. The balloon number filled in correctly.
It would seem that model or relative views of a weldment body both behave properly with a balloon number.
If you want linked note data, that works as well. There may be a more streamlined way to do it than this so please speak up:
Add a note to your relative/model view, select the "Link to Property" option in the property manager.
Select "Component to which the annotation is attached" in the Link to Property dialog and choose the property from the drop down.
If the cutlist property is not shown in the list, pick another temporarily.
Your note will show the data for the entire model - not the individual weldment body.
RMC on the note text and select "Edit Text in Window"
You will see something like $PRPMODEL:"Description"
Edit this to something like $PRPWLD:"Name"
Make sure the WLD is in caps.
I tried the ballon and it works. The lable would be great if I only knew what variable soldworks uses for the item #. I ended up using a note for the lable and clicking on the ballon to get the ID data for the item inserted into the note.
You could also do a Insert(drop down)->Features-> Save Bodies. to save off each solid body, or in this case cutlist items
These should be helpful
Assembly from Part – No mates required (convert multibodies to Assembly)
Detailing a Multibody Part-1
Detailing a Multibody Part-2
Exploding a Multi-body part -1
Exploding a Multi-body part -2
Good Afternoon Deepak,
I am curious about your link above - Assembly from Part - No mates required.
This process will take all bodies and make them all individual part files then form an assembly.
I am curious whether this option is available to follow this process, but instead of making all bodies in to individual part file to select multiple bodies for different part files. Similar to the functionality of "Insert in to new part..."
Grant, there is no option to select more than one body when using this option.
But you can have one part for the body having multiple instances in the part using the option highlighted in picture below.
Retrieving data ...