Solidowrks weldment bonding box with pattern features

[pllmoreau]

Hello,

I am making a weldment structure that has a lot of channels with the same distance between them (48in) I need to connect the channels to another beam with a plate so I made an extrude feature which solidworks recognizes in bonding box for my cut list as a plate in my 2D drawings. However I made a linear pattern of that plate so that I don't have to draw the plate for each channel but the bonding box does not recognize these plates for the cut list so it messes up the quantities in my 2D drawings, same goes for mirror features. Is there a way to include those features in the bonding box so that my cut list has the correct quantities. I am using solidworks 2017.

Thank you!

 

[Jboggs]

When you made the linear pattern did you pattern features or bodies? Which?

 

[drawoh]

pllmoreau,

When I attach flanges and plates to weldments, I use the equation editor to control the sizes. When SolidWorks sees six plates 100mm[×]136mm, with a 20mm[×]45[°][ ]chamfer in one corner, it will create a cut list item with six pieces.

I am surprised that the linear pattern does not work. I am generally very impressed by the weldment feature.

--
JHG

 

[Jboggs]

Again, are you patterning features or bodies? Which one? It makes a big difference.

 

[pllmoreau]

Hello,

sorry for the late reply, I was using pattern feature because I dont know why the pattern body did not keep the holes in my plates.

 

[drawoh]

pllmoreau,

When you extrude or rotate a sketch in SolidWorks, you have the option of integrating it with the existing part, or creating a new body. In a weldment, you need a new body. This is what Jboggs is referring to.

--
JHG

 

[Jboggs]

Patterning or mirroring features and bodies can be tricky, but once you understand it becomes second nature and it makes perfect sense. For example, cuts and holes are applied to bodies. You have a choice of WHICH bodies they apply to. Look in the cut feature properties box and you'll see an option for all bodies, or selected bodies, or automatically selected bodies. If you make a cut on a body and then try to pattern or mirror that cut to apply to other bodies it won't work because you originally declared that cut to only apply to the original body. However, if you originally selected ALL BODIES for that cut, then when you pattern or mirror it, it will apply to those new bodies too.

For an exercise that is a little weird, find at a part with at least two bodies. They don't have to touch. Pick a surface on one of the bodies for a sketch. Draw a circle for a hole that can go through both bodies. Extrude Cut through all. Let SW automatically select the bodies, or select ALL bodies. It made a hole all the way through all bodies. Now go back and edit that hole feature, only this time select only a body other than the one on which you drew the sketch. You can cut a hole through a body that is literally BEHIND the one on which you drew the sketch, without that hole going through the native body.

You can also play similar tricks with patterning and mirroring.

Hope this was all clear. Have a good weekend everybody.