Is there a way to set sheetmetal thickness of a base flange to the value of an offset dimension?
I don't want to have to set up a design table or global variable but associate the dim in sheet metal parameters to the 5mm offset dim that other components will be referenced from. I input "=" and click the sketch dim and no love.
You could link the offset dim to the Thickness global variable.
Double click the thickness to edit it. Then, proceed to write ''=#######'' where ###### represents your offset dimension that you will select.
Summed up:
Edit thickness
Write = in the dimension box
Click on the offset dimension in order to have it be added as an equation to your thickness. Should look something like '=@D3@Sketch2'
Voila, your thickness is linked to the offset.
or
Well it all depends on how he wants it to work.
From what I see, yours would be the thickness in the function that controls the offset in a sketch. Mine would be the offset in a sketch that drives the thickness in the function.
Hi Alex,
Thanks for that but that is my problem, it doesn't work. for most things you can do that and I frequently do but for sheetmetal thickness it asks for a specific number only unless using variables.
Thickness will be different for approx 24 parts in the assembly so I will need to add a prefix to the thickness in the global variables and this gets out of hand rather quickly. the best solution is as you suggest, to make the sheetmetal thickness ="offset dim@sketch" but it doesn't seem to allow this.
I've never used custom properties but I've heard of a lot of people overriding stuff being blocked by SolidWorks like this with these, perhaps it could work?
Deepak Gupta, John Stoltzfus , I think I've seen one of you two speak of custom properties
Also, perhaps you could try configurations for your different thicknesses and have them have configuration specific names to design your part number?
If you have time take a look here What are your most impressive tricks of solidworks, Please spread.
There is a bunch of posts regarding Custom Properties and Custom Property Tab Builder, you'll be surprised how easy it is once you get past the setup issues. No more typing multiple times in multiple places, auto fill drawings and BOM's
I tried to get Alex's method to work but it just wouldn't. May be a setting??.. What I did was to sketch the profile for the base flange, did the offset (construction) and selected base flange. At this point it doesn't matter what the thickness is,, just need to establish the global variable. Then made the dims show ( right click Annotations, show feature dims). Then did an (right click on dim) unlink value on the thickness dim. Then linked the two dims to drop down arrow thickness) FYI.. I had tried to link the two without unlinking the thickness dim but it will not allow that.
Then a rebuild. Then change the sketch offset dim to whatever.
Rebuild.
You can now change that value with the sketch offset. The original thickness dim.. Or in the sheet metal property manager.
Awesome, that works! I'll check to see it it works on an assembly level also.
Thanks!
Doesn't work on assembly level for my purposes unfortunately, Assembly level sketch shown below on front, right and top planes.
entities converted from assembly level sketches to make sheetmetal parts of differing thickness.
Sometimes a client will want to alter and currently its a 2-step process of altering offset dim in assembly so parts fit together well still and then change the sheetmetal thickness on the part level to match the assembly. not a major issue but good engineers are lazy and a 1 step process is far more efficient!
You are correct sir, I assumed it would work without trying, it is blocked because of the link you speak of. Your method is tops!
I tried to get Alex's method to work but it just wouldn't. May be a setting??.. What I did was to sketch the profile for the base flange, did the offset (construction) and selected base flange. At this point it doesn't matter what the thickness is,, just need to establish the global variable. Then made the dims show ( right click Annotations, show feature dims). Then did an (right click on dim) unlink value on the thickness dim. Then linked the two dims to drop down arrow thickness) FYI.. I had tried to link the two without unlinking the thickness dim but it will not allow that.
Then a rebuild. Then change the sketch offset dim to whatever.
Rebuild.
You can now change that value with the sketch offset. The original thickness dim.. Or in the sheet metal property manager.