I have a sheet metal part I'm trying to replicate in SolidWorks. I have the dimensions of the unbent, cut metal and want to sketch that and then add bends to it. Is there a way to add bends that subtract the necessary material from the metal already there? As it is now, when I add bends it adds material and screws up the original unbent dimensions.
Drew,
You can use "Sketch Bend" to add bends to a flat pattern. You will need to use the correct radius and k factor, bend allowances or bend deductions to get the same size part. It would be a lot easier if you could get the bent part, rather than the flat pattern.
Jerry S.
Seeing as how the flat part already has the bend allowances or deductions applied it could be relatively easy to determine what they were. If there are only two 90 degree bends on the part, you could just add the sum of the total outside flange dimensions from the flat length you have in the flat layout. Divide the difference by the number of bends and you have the bend deduction.
Set that value in the bend properties for the part. Now draw a sketch bend line where required using 1/2 the value of the bend deduction previously determined to 'offset' the position of the sketch bend line. Your part should form with the correct outside bends while also not changing the flat dimensions.
You can apply a BD, BA or K-factor to individual bends in SolidWorks. Adjust each accordingly to get the finished part dimensions.
You are just working the problem backwards.
I find that using BD/BA is easier then using k-factors for this type of exercise.
Cheers,
Anna
You will need to know what bend allowances that were used when the flat pattern was created then adjust the parameters to suit.