Tek-Tips is the largest IT community on the Internet today!

Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!

Register Log in
  • Congratulations MintJulep on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Flat Pattern Drawings that Agree with Layout by Hand 4

Status
Not open for further replies.
Tigerdawg

Tigerdawg

Mechanical
Joined
Aug 9, 2002
Messages
40
Location
US
I am trying to figure out how to adjust the sheet metal settings so the flat pattern dimensions agree with the dimensions I would use when laying out the part by hand. For example, a 2 x 2 (inside lengths) angle would be bent out of 4" wide sheetmetal for thicknesses 11 ga. or thinner. This is not what I get from a SW flat pattern.

What settings must I change?
 
Sort by date Sort by votes
You have to adjust your Bend Allowance, specifically your K-factors. I think SW defaults to .5 for this value, but throught trial and error within our fabrication shop, we have found that a K-factor of .434 works the best (for us).

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?
 
Upvote 0 Downvote
Try setting the material thickness to .001 for the flat layout
cliff
 
Upvote 0 Downvote
Do a help search within solidworks for K-factor. Within that topic you will see a formula: BA=P(R + KT) A/180. This is the formula that Solidworks uses to determine the bend allowance. Set the right half of this formula equal to whatever formula you use for bend allowance. Solve it for K-factor. If you change the k-factor to this new value in your models, you will achieve a flat pattern equal to what you calculated by hand.
 
Upvote 0 Downvote
The formula above didn't copy cleanly, the P is Pi. The rest are as follows:

BA = bend allowance

R = inside bend radius

K = K-Factor, which is t / T

T = material thickness

t = distance from inside face to neutral sheet

A = bend angle in degrees (the angle through which the material is bent)
 
Upvote 0 Downvote
This can also be found in SW Help.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?
 
Upvote 0 Downvote
We use bend radius and Kfactor, bend tables can be way over the top. If you are looking to force the flat to be a certain size you will probably need to set the bend radius about .0001 larger than the sheet thickness, and the kfactor can be set as low as solidworks will let you. If you are looking to fake it is probably easier to create a configuration and call it partx-flat and just trim your flat part to be the part you want.

The bend radius and k factor will give you an accurate formed part based on the flat it creates providing you use an accurate radius, the k factor can be achieved by experimenting. We use sever different groups of Bend Radius and K factor combos depending on the machine the parts will be formed on and the thickness of the material. For instance for a 20 gauge galvanized part we use a bend radius of .033 and a K-factor of .5 This gives us very accurate part when the parts are formed with Airbending on one of our presses.

A way to figure out what works for you is to cut an accurate flat to 10.000 x whatever width, then put three or four bends in it and draw the part in solid works exactly as it measures (with calipers). Flatten the model and check the size, if it does not measure 10.000 long in the flat model, adjust your bend radius first, it should be 2/3 the material thickness or more. Then when you get it close to 10.000 fudge around with the k-factor til it is exactly 10.000 in the flat model. Run several test parts like this for each material and machine you use (or hand bending method if that is what you are doing). The longer your test peice and the more bends you put in it the more accurate you will be able to set your variables up. Good luck and have fun it is tough at first but if you are going to be designing a lot of sheet metal, setting up your bend radii and k-factor will be worth it.
 
Upvote 0 Downvote
aamoroso gives some good advice. Every k factor situation I've seen is best done with a correlation to physical bends. We have found that this is also influenced by the type of material, i.e., aluminum and steel, with the same thickness, flange length and bend radius will have slightly different k factors.

The one thing I would differ from aamoroso's advice is with regard to the bend radius. The bend radius shouldn't be tweaked, it should be entered as the value of the nose radius of the punch. Generally the inside bend radius should be 1.5 times the material thickness, though this is often violated. Most sheetmetal shops will have a standard set of tools with bend radii of .030, .060, .090, etc. Make sure that you and the shop are using the same value. This too is often violated (the shops would rather use what's in the machine than change to what you've specified). However, you should be designing with standard radii. With that said, we specified the finished formed part, including bend radii. Our flat pattern drawings were provided for their reference only. They (the fab shops) were free to use the FP drawings however they wished, so long as we got the formed part we wanted.

- - -Dennyd
 
Upvote 0 Downvote
I have ultimately gone the route of Dennyd for my sheet metal needs. Early on my company used specifically one sheet metal shop and I attempted to get them to use the flats I provided. I used their formulas to derive the necessary k-factor the way I described above. It was fine and dandy until purchasing sought after alternated manufacturing sources (as well they should to get competetive pricing). Now with multiple manufacturers and all of them using different formulas (because their equipment is different as aamoroso pointed out), I am unable to provide accurate flats. So it goes. Now I just want the parts as I specified them in the details.

Fortunately it sounds like you have in house sheet metal fab. So you should be able to make the manufacturing process more efficient by integrating SW generated flats into your drawings.
 
Upvote 0 Downvote
Thanks everybody. I've got an idea of what I need to do.

We do have a small shop, but also send out some work. I'll just have to set it up for what I'm used to and mark the flat pattern as reference for shops that do things differently.

Thanks again.
 
Upvote 0 Downvote
One thing that may not have been mentioned or I missed it with all the information provided was the use of the Neutral Axis of the bend . This neutral axis does not always fall on the center of the thickness depending upon the thickness/bend radius.

If this is addressed above I couldn't understand it. I was just browsing the forum. If it is already addressed, sorry

Gerald Austin
Iuka, Mississippi
 
Upvote 0 Downvote
jlcochran

Thanks. The K Factor seems to have covered what I was getting at. I had a formula from an ASM handbook on forming that I used to calculate where the neutral axis was located but couldn't recall the K-Factor.

A great Link!



Gerald Austin
Iuka, Mississippi
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

drcole
  • Locked
  • Question Question
sending a flat pattern to a sheet metal shop
Replies
7
Views
916
ctopher
ctopher
Jawed62
  • Locked
  • Question Question
Solidworks VBA with custom property
Replies
2
Views
2K
Jawed62
Jawed62
V
Problem to open a .obj file with the textures visible on the model in Solidworks 2022
Replies
0
Views
64
victor andreevich
V
FranscoisMH
  • Locked
  • Question Question
Solidworks Automation: Creating a flat pattern drawing from a sheet-metal part with automatic dims
Replies
1
Views
913
SBaugh
SBaugh
LeRepeteur
  • Locked
  • Question Question
PDM Question - FileVault and Save As of Drawings and Assemblies
Replies
11
Views
1K
drawoh
drawoh

Part and Inventory Search

Sponsor

Back
Top