Is there a custom property value for "bend deductions"? I can't find it...
I want the drawing to include the bend deduction, bend radii, and such on my
drawings that go to manufacturing in our shop...
If I put in my bend table it would only confuse the machine operator
I guess I need to write a macro and have it extract it to the drawing...
i.e. make the drawing from the part and then run the macro to "stamp" the
bend deduction on the part... maybe I will add things like bend radii and
whatever else is needed as well in the same macro(?)
The problem is I do not know what the custom property (or even API command)
value gets me the bend deduction - or what ever is being used for the bends
on the part.
I use the two templates in the following links with great success.
They allow me to confirm correct stretch and convey relevant details
to the operators. The sheet calculates accurate bend deductions from
IBR, material thickness and angle of movement and those numbers are
verified against the STO of the flat pattern.
We normally use a k-factor of .445 to calculate flat patterns. For
press brake forming of steel from 22 ga to 1/2 thick it's normally
accurate to within .005". Occasionally we use .33 for dead-soft
material. What makes the most difference is using the correct inside
bend radii for the calculation. Bottom bending and air bending are two
different animals. If you are calculating layouts for stamping dies
for high volume highly accurate parts you should do trials of the
I don't include bend deductions on my prints - they are easy enough
for the operator to calculate from the flat length and formed
dimensions if needed. I do use SW standard bend notes with bend radius
radius and bend direction, and locate the bend line from the gage edge
for the operators.
When we started with SW back in 99 we were using an excel sheet to
calculate layouts. Until we proved out that SW was giving accurate
layouts we cut and pasted the excel table into the print; mostly as a
courtesy to inspection.
If I was going to put a note in the drawing with the bend deduction
I'd make a standard note for the design library, then drag the note on
the print when needed and just type in the bend deduction value.
The bottom section of the development sheet represents our brake.
Operators sketch in tooling set-up and then keep the sheet for future
Flat pattern is based on a bend table, which uses accurate IBR and
material thickness. It is embedded into our sheet metal part template.
The profile drawing template has the XLS embedded for checking the
stretch. IBR, material thickness and angles are entered and deductions
are calculated by formula (same formula in the bend table). Leg
dimensions are entered into the sheet in the dimension column and the
letter (A, B, C....) of the column of the worksheet which contains the
desired angle is entered. The letter is converted to the associated
bend deduction via macro. Entering a period (.) will insert the value
from column A, which is usually a 90=B0 angle. This allows for rapid
entry and reduces the possibility of typos. The green and yellow
background colors are added via macro and represent back gauge to
center of bend dimensions, which operators use for programming.
A flat pattern is inserted on tab2 of the drawing file and STO
dimensions are applied as shown in the next link. The STO dimensions
are linked to tab1 drawing format. The actual measure STO should match
the numbers in the development worksheet.
It takes much longer to explain than to actually do. I can typically
process a sheet metal component in less than 3 minutes. This includes
DXF flat pattern and profile detail for laser cutter, development
sheet and bend detail for brake operator and a shaded iso view for
reference. I have had zero errors in flat patterns for the last two