K-Factor for multiple folds

[cmundyLWUM2]

I am currently setting up Inventor for the sheet metal company I work for but have been encountering issues regarding the K factor. We have been unable to fold the attached test enclosure to anything close to the folded model. The below is using a standard 0.44 K-Factor in 1.5mm Zintec. We fold the front smallest folds first with an 8mm V, with the last folds being the 200mm ones. Consequence of this is that we are always out in the rear (400mm dim). We have tried both brake press settings of folding to internal dims and external but to no avail. 

My understanding is:

- that that smaller the K = the smaller the blank size

- the greater the K = the greater the blank size

This in theory would mean the 3mm we lose in the back would be gained with a larger K factor. However, Inventor sheet metal increases every fold and therefore throws it out. Any advice would be greatly welcome.  

[JDMather]

@cmundyLWUM2 

What version of Inventor are you using?

Attach your *.ipt file of the part here.

[cmundyLWUM2]

@JDMather we are on Inventor 2024 and please see attached.

[JDMather]

For each bend you might need to run a test and set an appropriate kFactor for that individual bend or set up by bend table rather than kFactor.

[Mario.VanWiechen]

nothing wrong with your K factor.

The bend radius that you are getting when you bend is what is throwing your numbers off.

You specified inside rads equal to material thickness, the 2 different dies you are using are giving you very different radius's thus skewing your numbers.

Die opening should be 8 x specified radius, or 12 mm to produce the bend radius you specify. The measurements will be much closer then

[swalton]

I have always understood that sheetmetal k-factors depended on at least 4-5 variables.

• Material
  • Sometimes including grain/rolling direction
• Thickness
• Punch Radius
• Die Width

When I have done high-precision sheetmetal work, I have had the sheetmetal shop provide k-factors or sample hat sections for each combination of the above variables.  I adjusted the model k-factor to match the real-world samples from the vendor.  You may have to do the same to get accurate blanks.

[Frederick_Law]

You need to find k for your tooling and process.

The k in Inventor is for reference only.

It is not "Standard".

[blandb]

Have you bent sample pieces in your shop and reverse engineered your k-factor? Have the shop cut a square and bend a sample as equal legs and reverse engineer the k-factor to see what it actually needs to be as a starting point. That way you will be creating an unfold rule that will make sure INV will be talking to your tooling for that sheet thickness. Maybe the K-factor is something other than the default standard. Maybe it actually comes out to be 0.2478 instead for example. Then you can back check different radii to see if you specify a specific radius that you will get a specific flat. Then in inventor if you apply a specific unfold rule to be used for that sheet and you can also choose for a specific flange to use a different unfold rule if needed via the unfold options tab in the flange tool.  I have only had a need to use uniform rads for our sheet stuff, so I have not actually applied a secondary unfold rule to a specific flange to see if it truly works that way. Just some thoughts

[Mario.VanWiechen]

The OP does not understand the consequence of the bend rads not matching the drawing. He is using a too small opening for some of the bends and a too large opening for the rest. The drawing requires a certain die opening or a smaller die opening with a radiused punch.

K factor is not the issue here, not understanding bending metal on his part and the part of his shop personnel

[cmundyLWUM2]

Thank you @Mario.VanWiechen we trialled the 1.5mm using the 12mm V and it worked great!

With this logic our 2mm will require the 16mm V. However, I notice the 1:8 ratio wouldn't work for say using 1.2mm in an 8mm V. Is there a calculation chart which determines what to adjust your internal radii to or is it trial and error?

Thanks again

[Mario.VanWiechen]

1.2 x 8 = 9.6, a 10 mm opening would be better.

a smaller opening will work but you need to have a punch with a 1.2 mm radius on it. Typical punch has a 1 mm or smaller rad

[cmundyLWUM2]

All the tooling has 0.6mm radius on them and are 88 degree. Thanks for your help.

[johnsonshiue]

Hi! If you want to see the flat pattern length equal to the inside perimeter or outside perimeter of the folded part, change the K factor to 0 or 1.

But as the experts already mentioned, the exact K factor to use depends on several variables.

Many thanks!

[cmundyLWUM2]

FYI the step file for relevant model.

[Mario.VanWiechen]

---

@cmundyLWUM2 wrote:

FYI the step file for relevant model.

---

No file attached

[cmundyLWUM2]

Apologies, please see attached.

[YannickEnrico]

I just want to reiterate

Unfolding in inventor is dependant on two things:
K-Factor and Bend Radius

Developing appropriate K-factor and Bend Radius settings would depend on real life observation of bend tests. For instance, bend a 100x100 blank 90 degrees, and see how it behaves.

My previous work place developed a bending table that way.

The way I have always worked with sheet metal is to keep a constant bend radius, BendRadius = Thickness.
That way I only have to adjust K-factor when unfolding.

Even if the part in reality has another bend radius, I use inner radius = thickness, because if I adjust for reality, my K-factor changes as well.

I'll attach a small tool I wrote that determines the K-factor based on thickness, radius and extension (how much bigger or smaller the part becomes during a bend)

Edit:

Maybe one of the native speakers can tell me what it's called? Bend addition, bend extension, bend allowance, or whatever. Those 10ths of a mm the material changes in length per 90 degree bend.

[Frederick_Law]

---

@YannickEnrico wrote:

Maybe one of the native speakers can tell me what it's called? Bend addition, bend extension, bend allowance, or whatever. Those 10ths of a mm the material changes in length per 90 degree bend.

---

Bend allowance, bend deduction.

Most shop has no idea what k is.

They have "rule of thumb" for 90 deg bend to remove a bit of material from total length of flanges.

Bending stretch material so it's always remove material.

Everything affect k, bend allowance:

Material hardness, strength, grain direction, heat treat, tempering, temperature when bending

Bend radius

Bend angle

Bend method, air bend, corning, stamping, rolling

k work well when bend radius is thickness or more.  Up to a certain size then it get into "rolling".

Bend table is best if you got different radius, die, operation on each bend.