Multi-Body Design Library Features

New for SolidWorks 2013 is the capability to store library
features as multi-body files.  This works
great for adding plates and mounting feet to weldment part files.  The process for making one of these library
features couldn’t be easier.  I’m going
to walk you through the steps for making a foot plate to insert inside of a
rectangular structural profile.

First you want to make a base extruded feature in a new part
to simulate the type of placement you will have for this foot plate.  Next you will model the foot plate and place
it inside of the first profile.  I have
also added some chamfer features that can be controlled at the design library
level as well as a tapped hole to allow fasteners at a later time.  

Be sure to make this second extrude its own body by unchecking the Merge Result box.

Second, you will choose to add this to the design library
folder of your choice.  Give it a name
and description for ease of use by your co-workers when they need to add this
to their designs.

Next, you need to edit this library feature and setup some
conditions.  In this image we are
choosing the references for placing the foot plate inside of the tube. 

I have a face selected for placement and 4
edges to allow this plate to grow and shrink based on the size of profile I am
attaching this to. 

Finally you need to
choose which dimensions are presented to the user and which ones are
hidden.  You do this by dragging
dimensions from the Dimension folder to either locating dimensions or internal
dimensions.  

Re-save the file and you are
on your way.  You can then use this in any part weldment that contains 4 edges to locate to.

Thanks!

Brian Reel
CATI 

How to: Add Full Standard Weldment Profiles

Multibody BOM With Cutlist

    So you’ve built this awesome set of cavity and core blocks with the Mold Tools in Solidworks.  You did everything in the right order.

• Imported your neutral file from your customer.


• Fixed up the missing geometry for molding (because there is always some thing not quite right)


• Added shrink.


• Parting line


• Etc.

 

Multibody Cavity Build

 

    Check, were all good. You get to the end of your workflow and you would like to show your “Multibody  Exploded view” new for 2012 and it works awesome!

    As a sideline it’s as easy as it is in the assembly. If you can’t find the command type into the search command box in the upper right hand of your SolidWorks window and look for the command. Drag it on to any toolbar you want. My rule is if I need it more than 2 times, it is going on a toolbar.

Command Search

 

    Back to the point of this discussion. I want to make a drawing with a top level BOM.  I take my multibody exploded view in isometric and I insert it into a drawing.

 

BOM as Multibody

 

    Problem here is after I insert my BOM…its parts only and since this is a multibody it calls it out as 1 part, 1 description. Boo Hiss!

1&1 yuk :(

 

 

 

 

 

 

 

    The good news here is you can turn anything into a weldment at any time. So at this point I want to leverage the cut-list functionality of the Weldment feature.  

Yeah Weldments!

       So now all you have to do is fill out the properties for the cut-list items that you want and reinsert your BOM. This time you have another option.So now all you have to do is fill out the properties for the cut-list items that you want and reinsert your BOM. This time you have another option.

So now all you have to do is fill out the properties for the cut-list items that you want and reinsert your BOM. This time you have another option.

Yeah!

    It works great and could be used in a top-level BOM of a completed mold assembly. The final results look like this.

Nice!

 Hope this helps,

 

Todd Werginz

Computer Aided Technology

Creating a view of a single structural weldment in Solidworks

If you create a structural member in Solidworks 2012 that has two or more members mitered to each, it causes the drawing view of that structural member to show all the members that are mitered together. The first picture that you see there was created using one structural member/one group.

However what if you wanted a drawing view of just one of those members and not all of them you would either have to split them up into multiple structural members or simply uncheck on the option for “merge miter trimmed bodies”. 

 

Then you will be able to create a drawing view of just one of them members.

 

Ketul Patel