Hi Dave,
Some years ago I looked at it.
To be very short about it;
The dialog is asking the questions that need to be the answered.
This is what the dialog looks like now:
I would rather see a dialog that asks me:
- Material Type
- Material Thickness (that is avalaible for the choosen Material Type)
- Bend Tool Setup (that is physically available AND functionally possible for that given Material Type/Material Thickness combination)
The result in the 3D Sheet Metal design should be a specific Bend Radius and Specific Bend Neutral Factor according to the bend angles that are present in the design.
btw Bend Radii tend to get bigger with larger inside Bend Angles.
As the dialog is now it is as if we can oblige the material to be formed with a bend radius as we would like. In reality this is not possible with air bending = press brake bending.
The only way of forcing a specific Bend Radius would be by "bottoming" -meaning that the punch forces the sheet metal plate fully down in the die- like stamping.
Since the existing dialogue can't do this I stopped investigating this any further and decided to do it our own way. (BTW it's the same method that e.g. Trumpf and LVD use. I bet there will be other press brake manufacturers that use the same method)
In general the design and the tools being used dictate what the resulting bend radii will be.
NOT the other way round. This is where almost any CAD system fails. In fact I don't think that there is a CAD system at this moment that does this correctly OOTB.
Maybe SWX in combination with an add on called TopsWorks.
And also TruTops Boost in combination with SpaceClaim.
Hi Ryan,
Correct; the dialog is asking for imput that I'm actually looking for.
Since a Bend Radius is the RESULT of a chosen Material Type - Material Thickness - Bend Tooling - designed Bend Angle, it seems rather strange to me that you need to provide a bend radius yourself.
Also given the fact that a bend radius tends to get bigger when the inside bend angle gets bigger.
Here are some random values that I've taken from our database (for a given material and tool setup):
Inside bend angle | Material Thickness | Bend Allowance | Back Gauge Correction | Inside Bend Radius |
| 90 | 2 | 3.75 | -1.875 | 2.15 |
| 105 | 2 | 2.59 | -1.295 | 2.38 |
| 120 | 2 | 1.77 | -0.885 | 2.72 |
| 135 | 2 | 1.15 | -0.575 | 3.38 |
| 150 | 2 | 0.67 | -0.335 | 4.91 |
| 165 | 2 | 0.28 | -0.14 | 9.67 |
Our database now contains almost 50000 lines and it will grow everytime we bend something new.
You might also notice the mentioning of "Bend Allowance " instead of a
"Neutral Factor"
I would also like to see the possibility to use a Bend Allowance for making bend corrections.
A Bend Allowance is a correction DISTANCE that you need to deduct from the sum of the desired outside flange dimensions. This means that this is a value that can be measured directly from a bend test. It is very direct and straightforward.
Working with a Neutral Factor always means that you need to calculate.
I hope this helps 
This group is dedicated to the discussion of Sheet Metal in NX.
