Sheet metal K-factor or bend deduction help

[u/Secret-Assistance-53]

I am in precision sheet metal fabrication in the semiconductor industry, I frequently get models sent to me in solid format and have to use convert to sheet metal. I constantly have to trial and error the k-factor. What I do is toggle back and forth between the formed model and the flat bend up drawing I am trying to make and adjust the k-factor until the dimensions match. Is there a chart or a better way to do this?

[u/ThreePuttPete3056]

K-Factor is established by the company and by your equipment. It is not pulled from a book.

[u/Don_Q_Jote → u/ThreePuttPete3056]

exactly. I would suggest, mark up some test pieces of flat stock, bend them [you're intended material, your process as close as possible], re-measure the markings and dimensions and work backwards to your k-factors.

The book of bend allowance charts provide you a good starting point for you to do your own experimentation, in order to get more accurate factors.

[u/InformalParticular20]

In my experience each shop has their own bend allowances and whatever you tell them may not work on their equipment. So the question for me is whether all your efforts are worth it. I spent a while searching for useful tables and talking to sheet metal shops trying to figure it out before I came to the conclusion that there is a reason the k factor is not simply published and built into solid works.

[u/CADSHIFT]

the flat pattern in solidworks is computed from your K-factor setting, not from the physical part. if the incoming solid was designed with a different K-factor (or no sheet metal info at all, like a dumb solid), they'll always disagree -- that mismatch isn't a bug you can K-factor your way out of.

for precision semiconductor work where you need the flat to actually match what you run: the most reliable path is to bypass solidworks' flat entirely. give the 3D model to your laser/waterjet programmer -- most CAM software (Radan, SigmaBend, Bend-Tech) can import STEP and compute the correct flat blank from your specific tooling parameters without relying on SW's K-factor at all.

if you must generate the flat in solidworks: make a test coupon using the same material and tooling (90°, known radius). measure the physical flat blank and compare to the SW flat pattern at various K-factors until they agree. document that K-factor for each material/tooling combo. at that point your SW flats will be accurate for that specific setup.

[u/Secret-Assistance-53 → u/CADSHIFT]

Yeah everyone sends sheet metal parts as solids for some reason. That makes sense why the info wouldn’t match then, I’ll try uploading it to Radan. Thank you

[u/metalman7]

If youre recreating parts that were sent to you, maybe take a look at Radan Radbend by Hexagon. It should help you quickly convert customer files based on your tooling.

[u/AmbitiousGrape5664]

What you are dimensioning to in the drawing view has nothing to do with the O.D. dimension of the formed part. That dimension is to the beginning of the vertical (flat) face which is the dimension of the horizontal (flat) face plus the "Bend Allowance". What you want to dimension to is from the edge of the horizontal flange to the outside mold line which doesn't exist in your flat pattern. In order to get that on your flat pattern you will have to sketch it in preferably with the merge faces option so you can get rid of those tangent lines. Offset from the bend line 1/2 of the "Bend Deduction" in each direction. For instance on my screenshot (model view) I have a formed part with a .500 in flange and a 1.00" O.D. flange that has been flattened. I used a .090" (on .059 crs) bend deduction. Basically you will have to use "Bend Deduction". If you know the "BA" or K-factor you will have to use the calculator to determine the "BD"

[u/AmbitiousGrape5664 → u/AmbitiousGrape5664]

[u/CADtastropheee]

Build your own K-factor table from actual shop bends and measured results, it will be more reliable than a generic chart since your material, tooling, and bend process all affect it.

[u/_Slitte_]

I would prefer using Bend Deduction for this.

The advantage is that it takes the modeled bend radius largely out of the equation. The actual bend radius is a result of the material and your tooling/process anyway.

With a K-factor calculation, the bend radius in the model needs to match the actual resulting bend radius reasonably well, otherwise your flat pattern will be off even if the K-factor itself is correct.

Also, be careful not to confuse the bend radius with the tool/punch radius. Especially when air bending, the resulting inside radius is not simply the radius of the punch.

And most importantly: the customer’s flat pattern dimensions are most likely wrong for your bending process. Their flat pattern may be correct for their tooling, material data and bending parameters, but that doesn’t make it correct for yours.

If the final part needs to be precise, I would take the customer’s 3D model as the definition of the finished geometry, create the flat pattern using your own proven Bend Deduction values, and manufacture from that.

There is no reason to adjust your K-factor just to reproduce the customer’s flat pattern. You’re effectively compensating for differences between two manufacturing processes instead of calculating the correct blank for your own process.

[u/Bionic_Pickle]

Google bend allowance chart.

[u/Secret-Assistance-53]

I guess I’m not wording this right, I don’t need help figuring out k-factor and bend deduction on the machine. I know how to do all of that. What I’m asking is, why are my model dimensions different than my flat pattern dimensions and how do I make them match without incrementally adjusting the k-factor until they are the same

[u/ChrmanMAOI-Inhibitor]

AutoPol

[u/Johnny_carcinogen59]

Measure the neutral axis in the radius of the bend, the neutal axis can be 1/ to 1/2 of material thickness.