SOLIDWORKS Weldments is a powerful function of SOLIDWORKS and can allow you to quickly and easily model weldment structures, Frames and beams that form the backbone of products developed by many industries. SOLIDWORKS Weldments quickly creates designs that have extrusions and generate cut lists and bills of materials needed for manufacturing. SOLIDWORKS accelerates the design process, saving time and development costs, and increasing productivity.
However when it comes to actually making those frames in real life, those tube ends AKA bird mouths can be a real pain to create and cut.
But don't worry! I thought i'd share with you a step by step guide of creating cardboard/paper cut-outs derived from your 3D CAD which you can wrap around you structural members to trace and cut those bird mouths out perfectly. You can create a library of commonly used wraps and just print them out when needed.
The first thing you'll need to do is open up a Weldment Structure. You may notice a few beams that have the same bird mouth shape, this could save you time because you will only have to create the Cardboard/Paper Wraps once rather than replicate the same one multiple times.
The next thing you’ll need to do is to save out the selected weldment bodies as individual parts. The reason we do this is that you can convert these into sheet metal parts, flatten them and get a Flat pattern or dwg/dxf that you can print and use for the wrap template. This is done by opening the Cutlist folder, selecting the items body, right clicking and selecting ‘Insert into new part’.
Once you have your individual structural member in it own part template you can begin the process of converting it into a sheet metal part that can be flattened.
The first and most important step of this is to sketch a profile perpendicular to the beams length. You will use this profile to split the structural member.
Now this bits important! You need to make sure that if the tube is circular that the profile is an angled from the centerpoint as shown in the image on the right. If this profile were not angled then the part will fail to unfold. This is different for flat faced structural members where a regular right angled cut is fine.
Extrude Cut this Profile through all.
Now You have the sliced part, You need to ‘Insert Bends’. This will convert the part to a sheet metal part and allow you to Flatten.
If you go into the ‘Insert Bends’ tool which is found on the Sheet metal tab and select the inside edge as shown in the image on the right. From here you can define bend angle and other paramaeter but for creating a Cardboard/Paper wrap these options are irrelevant.
Now you have a sheet metal part with a bend you can flatten and create a dxf/dwg that you can print 1:1 for our wrap.
The next thing you need to do is flatten the part. Click 'Flatten' in the sheet metal tools. This will flatten the part.
Once the part is flattened, if you right click the top face and select 'Export to DXF/DWG'. At this point you can create a location to store all of your wraps. For Export options select 'Face/loops/edges' and confirm. Click save.
The wrap will now be saved in the location you specified. You can either make a SOLIDWORKS Drawing of the flat pattern, print and cut out or you can use other 2D CAD software such as DraftSight and print from there.
Make Sure you print 1:1, otherwise your Wraps wont fit properly!
By Joe Baxter