AnsweredAssumed Answered

big bend angle mistake

Question asked by Mark Aranovich on Dec 17, 2010
Latest reply on Sep 5, 2012 by Bernie Daraz

Like • Show 0 Likes0
Comment • 19

Hi Everybody

I have problem with big bend angle.

As you see from attached file - it 20 degree angle, and SW don't want to unbend it...

Material- 16GA Stainless Steel (0.063") , as per my tables- for this material bend deduction- 0.1

When I put it- SW mark bend like mistake..

Wrote to SW support - receive answer :

"The only solution is to change the inputs for calculating the bend.

In this case it would be changing input for Bend allowance by either inputting a different value for Bend Deduction or using a different option such as K-Factor.

Increasing the Bend radius would also allow the bend to work. Adjusting material thickness may be a different option. "

Tried to switch from BD to k-factor (0.44) - not working

Tried to chage radius from 0.03 to 0.0625 (that tools which I have in metal shop)- same result.

Idea to adjust material thikness becouse SW can't calculate it is even not funny.

Please, let m eknow if somebody have REAL solution for this problen. I think, I'm not oly one , who need bend differnt , than 90 degree...

I need to receive real flat pattern, if I put numbers from the air SW will eliminate mistake, but flat pattern will be wrong...

Mark

Anna Wood Dec 19, 2010 3:05 AM

Correct Answer

The file Mark has uploaded has a k-factor of .46 for the entire part, not the .100 BD he talks about.

The 30 degree bend does not work with a .100 BD. Which is not a big surprise as I do beleive .100 BD is not a good number for that particular bend. I would adjust just that bend to a proper BD for a 30 degree bend.

Mark needs to do some empirical testing to come up with the correct BD for the 30 degree angle. Then create a SW Gauge Table for his material instead of hand typing in a number from his paper charts.

http://help.solidworks.com/2011/english/SolidWorks/sldworks/AllContent/SolidWorks/Core/Sheet_Metal/comb_Sheet_Metal_Gauge_Bend_Table.htm

The link from the SW Help shows that you need to add BD, BA for more then just the cardinal angles. SW can then more accurately interpolate the tweener angles.

http://www.screencast.com/t/ogQ29VWsL

The video shows that you can edit individual bend features for k-factor, BD, BA, etc, to override the global k-factor, BD, BA, etc set in the SheetMetal2 feature at the top of the feature manager.

Cheers,

Anna

See the reply in context

Attachments

FRONT DOOR.zip443.3 KB

No one else had this question

Outcomes

19 Replies

Kelvin Lamport Dec 17, 2010 7:39 PM
Mark Correct
Correct Answer
Fillet2 cannot exist within a sheet metal part. A sheet metal part has to be a constant thickness, and having a fillet or chamfer breaks that rule.

Drag the Fillet2 feature below the Flat-Pattern2 feature.
Like • Show 0 Likes0
Actions
Deepak Gupta Dec 18, 2010 12:47 AM
Mark Correct
Correct Answer
Mark I second what Kelvin has advised. And even I don't about a process that can add a fillet on the edge (like in your model) in blanking operation.
Like • Show 0 Likes0
Actions
Anna Wood Dec 19, 2010 1:20 AM
Mark Correct
Correct Answer
You can calculate what the material you are using needs for k-factor, bend deductions, etc based on your tooling and processes.

http://www.ciri.org.nz/bendworks/

http://www.ciri.org.nz/bendworks/bending.pdf

The pdf will explain how to reverse engineer your k-factor based on actually test bending the material you are using.

The BendWorks program is a neat tool to help you with that.

Cheers,

Anna
Like • Show 0 Likes0
Actions
- Kelvin Lamport @ Anna Wood on Dec 18, 2010 11:19 PM
  Mark Correct
  Correct Answer
  Well, that's weird. It flattens for me now also (SW2011-SP1, XPx32), but it wouldn't when I first tried.
  
  Any idea when the ability to flatten with a chamfer or fillet was added?
  Like • Show 0 Likes0
  Actions
  - Deepak Gupta @ Kelvin Lamport on Dec 19, 2010 1:23 AM
    Mark Correct
    Correct Answer
    Kelvin Lamport wrote:
    
    Well, that's weird. It flattens for me now also (SW2011-SP1, XPx32), but it wouldn't when I first tried.
    
    Any idea when the ability to flatten with a chamfer or fillet was added?
    Same here on SW2011-SP1, XPx64...
    Like • Show 0 Likes0
    Actions
- Anna Wood @ Anna Wood on Dec 19, 2010 1:36 AM
  Mark Correct
  Correct Answer
  I looked at your part as well...
  
  I am going to assume you have done real world testing and know your BD for your material and tooling at 90 degrees of bend based on the fact you said you looked at your chart.
  
  Have you added BD data into your charts for bends other then 90 degrees, 15, 30, 45, etc?
  
  The bend fails in the flat state most likely because SW can't calculate what is required. .100 BD is to much material for your 30 degree bend and SW does not have enough info to calculate what it should be at 30 degrees. .100 BD is only good for 90 degree bends. You will have a smaller BD for the smaller angle you are using for that bend that has an error down in the Flat-Pattern feature.
  
  You can go into your BaseFlange2 feature (click on the plus sign) and edit the individual bend features k-factor, BD, BA, etc.
  
  Do some empirical testing of your materials at the bend angles other than 90 degree. Add that info to your bend tables. Use that info for your 30 degree bend.
  
  After you have all your data be sure to create gauge tables that SW can use directly for generating the BD. Look up Gauge Tables in the SW Help.
  
  http://help.solidworks.com/2011/english/SolidWorks/sldworks/AllContent/SolidWorks/Core/Sheet_Metal/comb_Sheet_Metal_Gauge_Bend_Table.htm
  
  Cheers,
  
  Anna
  Like • Show 0 Likes0
  Actions
Jesus Vargas Dec 19, 2010 2:06 AM
Mark Correct
Correct Answer
I dont know but am I missing something here on this topic. I just open this file and I unfold it right away. so What am I missing?
Like • Show 0 Likes0
Actions
- Anna Wood @ Jesus Vargas on Dec 19, 2010 3:05 AM
  Unmark Correct
  Correct Answer
  The file Mark has uploaded has a k-factor of .46 for the entire part, not the .100 BD he talks about.
  
  The 30 degree bend does not work with a .100 BD. Which is not a big surprise as I do beleive .100 BD is not a good number for that particular bend. I would adjust just that bend to a proper BD for a 30 degree bend.
  
  Mark needs to do some empirical testing to come up with the correct BD for the 30 degree angle. Then create a SW Gauge Table for his material instead of hand typing in a number from his paper charts.
  
  http://help.solidworks.com/2011/english/SolidWorks/sldworks/AllContent/SolidWorks/Core/Sheet_Metal/comb_Sheet_Metal_Gauge_Bend_Table.htm
  
  The link from the SW Help shows that you need to add BD, BA for more then just the cardinal angles. SW can then more accurately interpolate the tweener angles.
  
  http://www.screencast.com/t/ogQ29VWsL
  
  The video shows that you can edit individual bend features for k-factor, BD, BA, etc, to override the global k-factor, BD, BA, etc set in the SheetMetal2 feature at the top of the feature manager.
  
  Cheers,
  
  Anna
  Attachments
  - Flatten_Fail.png735.0 KB
  Like • Show 0 Likes0
  Actions
  - Jesus Vargas @ Anna Wood on Mar 5, 2012 1:25 AM
    Mark Correct
    Correct Answer
    Oh ok But I still dont get it. does he wants to fight with the program or he just wanted to get it right because if he wants to get it right he can just switch it to k factor instead of bend table. I personally dont use the bend tables for many reasons. I work in a sheet metal shop and I unfold severals parts a day, and everytime I get a part from my customers if has bend table I just fo ahead and switch it to a k-factor. and just a little secret here. I use .398 as k factor and i'm always right on it, regardles of the angle and ofcourse in order to check if its correct your flat lay out, you have to know the real k factor. wich can be check with the sheet metal bend program that you posted yesterday. but I have to say that some of the calculations are way off. acording to my actual test on a fisical parts. but at least you can use it as a guide line.
    Like • Show 0 Likes0
    Actions
    - Anna Wood @ Jesus Vargas on Dec 19, 2010 7:00 PM
      Mark Correct
      Correct Answer
      Jesus, I agree you should test material and develop your own k-factors and BD based on your material and tooling. I bend metal as well. We regularly work to +/- .002 for forms. I use K-factors most all the time, especially for any bend that is not 90 degrees. We also have a good handle on what we need for k-factors based on real world testing, not rules of thumb. I would not use BendWorks factors. I would use BendWorks to do the math for reverse engineering a tested part to get real BD. Saves on doing the math.
      Like • Show 1 Like1
      Actions
  - Mark Aranovich @ Anna Wood on Dec 19, 2010 9:49 PM
    Mark Correct
    Correct Answer
    Thank you Anna and all, who help with this question.
    
    My problem, that 90% of our production is 90 degrees angle
    Very rare have different angles, and in this situation sometimes stuck.
    Is I already understand, is much better to use K-factor.
    I will calculate it according my BD table.
    
    Does somebody know good source for SW Sheet metal practice?
    I’m working wit several subcontractors, and every one of them has his own “secrets”
    One of them , use his own BD tables, another one just told me to use as BD- thickness of material, and swear, that always receive right parts.
    Sometimes, I think, that it sort of “everyone secret”, how to make parts in sheet metal.
    
    But does somebody know the recourse or book with this “secrets”?
    
    Mark
    Like • Show 0 Likes0
    Actions
    - Anna Wood @ Mark Aranovich on Dec 19, 2010 10:05 PM
      Mark Correct
      Correct Answer
      No, it is not better to use k-factor over bend deductions or bend allowance or gauge tables. All are valid if you have the correct data for your material and manufacturing practices. All, with the correct data, will generate very accurate flat blanks.
      
      Do you manufacture your parts in house?
      
      If not do not supply flat patterns to your suppliers. It is your suppliers job to figure out what they need and deliver you formed parts to print. If they can't generate their own flat patterns for the formed parts they deliver to you then you should consider finding different vendors who can.
      
      When we get flat patterns from customers we ignore them. We will calculate what we need for flat patterns to manufacture parts to print.
      
      Sheet metal is a bit of black magic at times. Do a search on Amazon for books on Sheet Metal. There is not one magic list of k-factors and BD that will work in all situations. What you need will come with experience and time in the field.
      
      Cheers,
      
      Anna
      Like • Show 1 Like1
      Actions
      - Mark Aranovich @ Anna Wood on Dec 19, 2010 10:27 PM
        Mark Correct
        Correct Answer
        Anna, my problem , that we manufacture parts in house, but when we "overfloated" we sent them outside.
        As well, most of StSt parts we also sent outside.
        For that reason we have 2 draings- one flat pattern with all dimensions and another one with bending dimensions only.
        When I sent parts outside, I have to sent them both drawings, otherwise they can't build the parts.
        Like • Show 0 Likes0
        Actions
Mark Aranovich Dec 20, 2010 9:34 AM
Mark Correct
Correct Answer
Following discussion I tried to calculate K-factor according
http://www.ciri.org.nz/bendworks/bending.pdf book

and also check muself according bend calculator from sheetmetalguy
Bend angle - 150 , thikness- 0.063, radius 0.063, BD 0.108

All the time I received values bigger , than 1.

According bending book "remember, most of the programs only accept k-factor values from 0 to 1"
What I need to do in such situation?

As well, today I received answer to my problem from SW support tem, and they suggest to use K-factor=4.0

Sorry, but I completly confused.According book, all k-factors plays around 0.4.

What to do in situation, when after calculation I receive bigger numbers, and how SW will deal with it?
Like • Show 0 Likes0
Actions
- Anna Wood @ Mark Aranovich on Dec 20, 2010 9:42 PM
  Mark Correct
  Correct Answer
  Look at the entire number in the output box that BendWorks shows you. It is likely something like 1.0234-E2. Put your cursor in the box and highlight the entire number and copy out.
  Like • Show 0 Likes0
  Actions
  - Mark Aranovich @ Anna Wood on Dec 20, 2010 12:06 PM
    Mark Correct
    Correct Answer
    Anna, sorry to desturbing , but how did you received this number?
    
    I receive different once (see attached)
    
    Can I put in SW k-factor greater than 1?
    Attachments
    Capture.PNG40.7 KB
    Capture2.PNG10.1 KB
    Like • Show 0 Likes0
    Actions
    - Michael Nelson @ Mark Aranovich on Dec 20, 2010 12:59 PM
      Mark Correct
      Correct Answer
      I can't open your part to check, but from the picture it looks like you are entering the wrong bend angle. It should be 30 degrees and not 150.
      Like • Show 0 Likes0
      Actions
    - Anna Wood @ Mark Aranovich on Dec 20, 2010 9:45 PM
      Mark Correct
      Correct Answer
      Mark,
      
      Michael has stated your issue...... Do not use the 150 degree angle, use 30 degrees.
      
      Then place your cursor in the Bend Deduction box and use your arrow keys to move all the way to the right to see the scientific notation.
      
      Cheers,
      
      Anna
      Like • Show 0 Likes0
      Actions
Bernie Daraz Sep 5, 2012 8:56 AM
Mark Correct
Correct Answer
This is an old post but it just popped up in the "More Like This..." box for me today. I understand the reason he entered 150 for the bend angle, or at least I know why he may have. There had been another more recent post on using the CNC control angle in a bend table also causing errors, though they also didn't realize they did this at the time.

Typically on Amada press brakes you enter into the CNC control the complement of the bend angle. For a 45 degree bend you enter 135 degrees into the control. For a 90, just 90. The print bend angle is entered into the CNC control as subtracted from 180.

Why they did this I'll never know, I never asked. I will someday. For now just accept it as fact. In sheet metal we've also had to deal with the fact that CNC program angles are not the same as tool load angles.
Like • Show 0 Likes0
Actions

big bend angle mistake

Attachments

Outcomes

Attachments

Attachments

Related Content

Recommended Content