Flat Patterns in SolidWorks

[majora]

Hi everyone, I'm new to solidworks so please bare with me. I'm running SW 2006 in my work place, and I would like to know how precise the flattening command in solid works really is. I work with sheet metal and I need to figure out flat patterns for a lot of parts, I'm hoping that SW can cut the time it takes me to figure out the bigger parts with multiple bends. I figured out how to flatten the parts, that's no problem, but I still need guidance as to how to use it right and if I can trust the flat pattern it gives me to put into production. Could someone please explain to me any tips, tricks, or point me to a website with good info on the subject. Thank you.

 

[CorBlimeyLimey]

You can select the type of calculation to produce the bends. (Bend Table, K-factor, Bend Alowance, Bend Deduction). See the SW Help file index for bend for details.

So to answer your question, the flatten function is as accurate as you care to make it. Lofted Bends being an exception.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[yanceman]

Majora,

I use SW to make sheetmetal formed and blank parts daily. I use a K-factor of .5 and a bend radius of .015". I add a derived configuration of the formed part for my blank. I select "Flange Outside" for the flange position selection when adding edge flanges. The guys who run the press brake tell me the formed parts are very accurate to the print. We use aluminized steel with thickness ranges from .036" to .057".

Yanceman

 

[MadMango]

Search these forums, this topic has been beat to death over the years. Also, SW Help is very useful.

You will also have to work with your sheet metal operators and see what type of tooling they use, what type of bending operations they are doing, etc.

We work with thicker materials, usually on the order of .105" to .194" HRPO and SST. Through a few weeks of trial and error, we found that a K-factor of .434 with bend radius of .063 worked the best for our operations at getting the physical parts to match the models.

[green]"Art without engineering is dreaming; Engineering without art is calculating."[/green]
Steven K. Roberts, Technomad
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[CorBlimeyLimey]

http://www.solidworks.com/swexpress/pages/nov05/TT_Sheetmetal_Tips.html

http://www.solidworks.com/swexpress/sept03/200308_techtip_02.cfm

Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[berkshire]

majora (Industrial)
Whilst you will find that the Solidworks flattening function and bend allowance program is very accurate,you have to bear in mind that the calculated dimension is only good for the material thickness,bend radius, and metal hardness that you have calculated.
If any of these values change, the result will not be what you intended.
If you are drawing for "in house" parts, draw up several small angles say 2" (50mm)by 2" with radii specified by you. Get your Brake operators to bend these as accurately as they can. Then measure them, note the errors and use this information to fine tune your K factor on your SW program. This is sometimes called reverse engineering the K factor.
When you are shipping drawings to an outside vendor send him a drawing of what you want made. Let him figure it out. If a flat pattern is included, it should be a reference drawing only.
I will now step off the soap box,
B.E.

 

[dogarila]

In my case, we are bending stainless steel, 12, 14 and 16 Ga mostly. For bendings with small radii I am using a bending radius of 0.001" and a k factor of 0.18. These values are quite strange but the flat pattern is accurate and the bent part matches the drawn part dimensions with the exception of the bending radius wich is larger in the actual part. For rounding I am using a 0.5 k factor.

 

[majora]

Thanks! These are all good tips. Let me explain a little bit about what I do, because I think my job may differ from what's being explained above. I create geometry for a CAD/CAM program that writes NC code to run our Laser and Plasma. I don't actually make drawings for the guys on the floor or at another company, sometimes I do when it's needed. I know all our tooling for the Break Press we have, plus I can run the machine if needed. So as you can guess I've got a good idea about the bending process, and for a little over a year I've been figuring out flat patterns using and excel spreadsheet that does the math for me to figure out BA plus the flat lengths. We bend plate anywhere between 16 Ga. up to 1" with radius's ranging from 1/32 up to 2.5". So I suppose what I do not understand in SW is what is the best way for my case to use, and how I should set the configurations up...

 

[CorBlimeyLimey]

Many sheet metal shops prefer to create their own flats from the formed drawings supplied to them. If you can figure out the flat patterns from the formed part model using your Excel spreadsheet, then you don't need to worry about the flat pattern output from SW.

If you are wanting to save yourself some time & work by having SW create the flat for you, then as mentioned above, all you need to do is select an option (K-factor, Bend Alowance, Bend Deduction) & input what works for your shop.

You dont have to worry about creating configurations, the flat config is created automagically.



Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[ctopher]

IMO, it sounds to me the best bet for you is trial & error.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[yanceman]

Berkshire,

Your method is exactly what we did here. Take a piece of pre-measured stock, put a 90° bend in it, take measurements again, etc... Our material thickness range is minimal, so one setting for all thicknesses works. The machine screw hole clearances will more than make up for a couple thousanths difference here and there.

Yanceman

 

[majora]

Thank you everyone for your input. I have a better understanding about the issue.

 

[berkshire]

majora (Industrial)
I happen to do what you do,I make patterns for an NC router.
We used to do what you do with Excel.
Now we just let Solidworks generate the flat pattern,then use an NC code generator called CAMWORKS to create the G code file for the the router.
B.E.

 

[Nella95]

Whew, buddy, SW makes flat patterns sooo much easier.

 

[keepinitcool]

The way I do it with the current metal shop I work with is to use the K factor and bend radius that they have come up with. They basically bent various test samples to determine their value. The values vary for ranges of metal. The benefit of using a fairly accurate bend radius value is that the metal will appear on the model with that radius, so if I want to know if the metal is contacting something else or needs to match to another part I can see that in the radius. If you just put in values that give the right flat pattern, the radius on your screen may not represent the curvature at the bend.