Help Please - Bend Deduction on Drawings?

If You use a bend table You can embed it (excel spreadsheet) into the SW drawing

// Krister

Hi,

If I put in my bend table it would only confuse the machine operator unfortunately...

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.

Thanks,

Aron

How was all the data calculated? is it a macro or table in SW. And what do the 2 views on the bottom represent?

Steve R

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 parts.

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.

regards, Diego

The bottom section of the development sheet represents our brake. Operators sketch in tooling set-up and then keep the sheet for future runs.

Flat pattern is based on a bend table, which uses accurate IBR and material thickness. It is embedded into our sheet metal part template. See link:

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 years.