K Factor on Sheet Metal Convert problem

[Normsthename]

I have been given some solids that I need to convert to sheet metal in SW2011
I have never used the convert tool before and I am having a small problem.
I managed to convert the solid to a sheet metal part easily enough.
But I cannot adjust the K Factor to achieve the correct blank size.
Solidworks is ignoring the K Factor, no matter what K Factor I input, the blank size remains the same
I also tried using Bend allowances etc but no joy.
I can get the correct blank size by adjusting the bend radius, but this is not ideal.
Any ideas what I need to do?

Thanks

Andy

[APinSoFla]

Can you send a sample file that's having this problem?

[Normsthename]

Here is a simple file that I created that shows the problem.
The flat pattern with a 2mm Bend Radius measures 47.75mm / 97.75 a total of 145.5mm
With the machinery available I want to achieve 47mm / 97mm a total of 144mm

The only way I can achieve 47mm / 97mm is to change the bend radius to 5.5mm, this is not ideal
Changing the K Factor has no effect.
I hope I have explained myself :)

Thanks

Andy

[JerryFlyGuy]

IIRC there is some glitch w/ 'convert sheet metal' that the K factor is locked at 50%. Same w/ lofted bends [again IIRC]. Have you talked to you tech support ppl?

I did some numbers w/ an actual sheet metal part and the needed K factor would be 0.184 but thats kinda a useless K factor, unless your bending a bonded bi-metal material or something.

A part that has inside dim's of 47 x 97, shouldn't [in reality] have a flat pattern of the same dimensions. The radius and k factor [which is 'right' to be at 0.50 [well 0.47 is a better number, but that would be splitting hairs].

Why not just shorten the original part to 'tweak' the flat pattern numbers so they line up it's all a 'fudge' at this point anyway!?!?

**Edit** remembered that 'lofted bends' calculates the K factor at the sketch location [so if the sketch is to the inside, that is here the 'center' of material is calculated]..This means that to get a 'perfect' flat pattern of a lofted bend, you need to draw your sketch at the 50% point of the material of the part [if that makes sense]

If anyone cares.. [didn't want to post incorrect info]

[Normsthename]

IIRC there is some glitch w/ 'convert sheet metal' that the K factor is locked at 50%

That's the conclusion that I came up with
Hope they fix it in an update

A part that has inside dim's of 47 x 97, shouldn't [in reality] have a flat pattern of the same dimensions.

Worked for me in the last 20+ years of sheet metal design! It all depends on the machinery / Tooling used.
It is near enough on materials upto 3mm, anything above that I calculate the bend allowance.

Thanks

Andy

[JerryFlyGuy]

Andy your right it 'works' but did you measure the parts afterwards w/ a caliper? I've been involved in building super heavy stuff out of formed plate and have gone as fine as building 20 gauge electrical enclosures. To have stuff that mates perfectly [ie fits into a jig for robotic welding etc] you have to follow the rules.

Now, having said that if you asked the average guy on the shop floor they will tell us to use inside dimensions and it's 'close enough'. Which for the most part is true [some might tell you inside dim's plus 1 material thickness]. Of course a welder can 'make' it all work by tacking parts together at dimension and then filling on a weld.

Lots of shops don't use a Brake that has an automated back gauge so then it really doesn't matter which formula a person uses it will be 'close enough', as thats all you'll ever get. If your using a CNC Brake w/ accurate top die positioning as well as accurate back gauge positioning and good condition dies, a person can tighten up those tolerances ALOT.

Again on a 10ga [or 3mm] part it's splitting hairs for a 'floor guy', not so much on something that NEEDS to be exactly to dimension [or a very tight tolerance].

Fwiw

[APinSoFla]

I deleted the "Convert" feature on your part and used "Insert Bends" and the flat pattern changes with K.