When in drawing space and placing a flat sheet metal part it automatically places bend lines what do they represent “start, center or end of bend”??? will these bend lines work for press, leaf or box brake ???
There are likely to be cleverer people out there but my guess is centre of bend. You could try and work it out by measuring from the outermost line to the edge of the sheet and compare it to the dimension of the end flange on the folded part. This should hopefully give you an idea, especially if you are using bend deduction and have the value. If not using bend deduction, and all bends are at the same angle, then add up all of the flange widths (outside face to outside face). Take this value and take away the size of the flat sheet, then divide this answer by the number of bends. If the measurement of the outermost bend line to the edge of the flat sheet is the same as the edge of sheet to the outside face of the first bend minus half of the value you worked out, then the bend line is centre of bend.
If inside your sheet metal model you check the flat pattern merge box, then the bend lines will be the centers of the bends. If the merge box is unchecked, then the bend lines will be the boundaries of the bend region.
Where is this located, searched in help but nothing
RMB on the FlatPattern feature at the bottom of the tree and Edit the feature. You can Merge Faces there.
The two lines are only representations of the start and end of the bend region. If you enter a fixed or otherwise known bend deduction (during modeling) the lines will not represent that number. IMO that is wrong and should be an insult to SW as they seem to want to do everything right. Back in the days of manual layout using Dykem and scribed lines you could check the flat pattern without doing a ton of math just by measuring to the lines as they accurately (for scribed lines) represented the actual bend deductions.
Depending on the type of bending you're doing I'm sure you can develop an 'offset' dimension to aid you in setting up your equipment. Obviously if you only have the one line and it is at the center of the bend it's almost easy to place your punch tip at that line for conventional ram type brakes and sharp 90 (or 88) degree punches.
Other than that the punch centerline is placed at the centerline of: length of flange minus one half the total bend deduction.
------- Sorry! ---------
The bend lines do indeed represent the bend deduction/allowance zones! I was referring to a part not done by yours truly. After checking the part to correct the k-factor to a bend deduction I found that I was incorrect in my earlier statement. Mea culpa!
The end result is I now have even more respect for SolidWorks!
Message was edited by: Bernie Daraz
Good morning Reno,
One way to double check your bendlines, (if they are centered or not), is to Right Click on the flat pattern view in the drawing and select tangent edges visible. That will show the tangent edge right next to the bend region.
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