Community
Hi All,
Please excuse me if this type of problem has been posted before, but I'm yet to find an answer to my problem without modifying K-Factor ratios etc. etc.
I've attached my "hollow bar" file and the screenshot of the flat pattern length where Inventor says the length will equal 4026.98 mm. If I manually (and roughly) calculate the length, I get plus minus 4066 mm. This shortfall would be extremely costly to us. I have confirmed the length with our supplier who also agrees with my calculations.
Am I not understanding Autodesk Inventor's sheet metal capabilities or is there in deed a flaw or limitation in the function?
Thanks in advance!
Lance
Hi All,
Please excuse me if this type of problem has been posted before, but I'm yet to find an answer to my problem without modifying K-Factor ratios etc. etc.
I've attached my "hollow bar" file and the screenshot of the flat pattern length where Inventor says the length will equal 4026.98 mm. If I manually (and roughly) calculate the length, I get plus minus 4066 mm. This shortfall would be extremely costly to us. I have confirmed the length with our supplier who also agrees with my calculations.
Am I not understanding Autodesk Inventor's sheet metal capabilities or is there in deed a flaw or limitation in the function?
Thanks in advance!
Lance
Accepted solution
No problem. The inventor counts correctly.
Your K-factor is set to 0.44. This means that there is a neutral bending axis at this height.
If you set the K-factor to 0.5, you'll get a manual result; because you were probably counting on it.
The K factor is responsible for the position of the neutral axis and, consequently, for the length of the arc.
It cannot be ignored in the design process and at the same time demand accurate results.
One follows from the other.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
No problem. The inventor counts correctly.
Your K-factor is set to 0.44. This means that there is a neutral bending axis at this height.
If you set the K-factor to 0.5, you'll get a manual result; because you were probably counting on it.
The K factor is responsible for the position of the neutral axis and, consequently, for the length of the arc.
It cannot be ignored in the design process and at the same time demand accurate results.
One follows from the other.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
You chose K=0.5 for your calculations. And you defined it differently in Inventor. Hence the discrepancy in the results.
The K factor should be selected - for technology, tools, etc. You will find information on the selection of the K factor on the web.
Once you choose it, you have to define it in the program. Inventor then calculates the length for the given factor.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
You chose K=0.5 for your calculations. And you defined it differently in Inventor. Hence the discrepancy in the results.
The K factor should be selected - for technology, tools, etc. You will find information on the selection of the K factor on the web.
Once you choose it, you have to define it in the program. Inventor then calculates the length for the given factor.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
No. In no case. This is part setup. You define once and use this file until the end (don't forget to save the file after changing the settings).
If you know you have a lot of parts with the same factor, you create a template and use it without searching and changing in each new part.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
No. In no case. This is part setup. You define once and use this file until the end (don't forget to save the file after changing the settings).
If you know you have a lot of parts with the same factor, you create a template and use it without searching and changing in each new part.
Kacper Suchomski
YouTube - Inventor tutorials | WWW | LinkedIn | Instagram
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
The inside length of your finished part is 3750.56mm
The outside length of your finished part is 4378.8mm
@lancermandc_co_za wrote:
I get plus minus 4066 mm.
I trimmed the Rip from my sketch of the centerline in image below.
When you bend a piece of metal the material compresses on the inside of the bend and stretches on the outside of the bend. In this case the difference between outside edge and inside edge lengths is 628.2mm.
The centerline measures to 4064.72 length.
See the Length values in each of these screen captures from your actual part.
But the neutral plane - where the material neither compresses or stretches is generally not at the centerline of the thickness of the material. The neutral plane is offset to one side or the other of the centerline. (Or from inside edge of the bend.) The k-factor.
This is also referred to as Bend Allowance or Bend Deduction (to account for stretching) depending on how the difference is calculated.
The Bend Allowance depends on
1. The material properties.
2. The thickness of the material.
3. The (inside) bend radius.
4. The bend angle....
and to a certain extend
5. The process used to create the bend.
For most parts the tolerance is not very critical and we can use a generic k-factor considering 1-4.
For critical tolerances we actually run a test piece and calculate and record a Bend Allowance table. This can very over time. In fact, we can set up identical machines to run the identical part and have a different Bend Table for each machine. As the machines get older - running test pieces and recording Bend Table becomes even more important.
For something like this I would definitely run a test piece to determine k-factor to use, but the Machinery's Handbook has some reference formulas.
The inside length of your finished part is 3750.56mm
The outside length of your finished part is 4378.8mm
@lancermandc_co_za wrote:
I get plus minus 4066 mm.
I trimmed the Rip from my sketch of the centerline in image below.
When you bend a piece of metal the material compresses on the inside of the bend and stretches on the outside of the bend. In this case the difference between outside edge and inside edge lengths is 628.2mm.
The centerline measures to 4064.72 length.
See the Length values in each of these screen captures from your actual part.
But the neutral plane - where the material neither compresses or stretches is generally not at the centerline of the thickness of the material. The neutral plane is offset to one side or the other of the centerline. (Or from inside edge of the bend.) The k-factor.
This is also referred to as Bend Allowance or Bend Deduction (to account for stretching) depending on how the difference is calculated.
The Bend Allowance depends on
1. The material properties.
2. The thickness of the material.
3. The (inside) bend radius.
4. The bend angle....
and to a certain extend
5. The process used to create the bend.
For most parts the tolerance is not very critical and we can use a generic k-factor considering 1-4.
For critical tolerances we actually run a test piece and calculate and record a Bend Allowance table. This can very over time. In fact, we can set up identical machines to run the identical part and have a different Bend Table for each machine. As the machines get older - running test pieces and recording Bend Table becomes even more important.
For something like this I would definitely run a test piece to determine k-factor to use, but the Machinery's Handbook has some reference formulas.
HI!
The standard factor in inventor (0.44) is an empiric standard starting value.
Despite the k factor selected, what really matters, is your final goal, and this is depending on several factors.
Different conditions (Fabrication processes, thicknesses, material, etc ), would give a different final result using the same flat pattern size extends.
The proper to achieve the correct kFactor is to do some real controlled samples: starting from a flat pattern calculated with the standard k factor and measuring the final result.
Based on these tests, it's possible to refine the proper Kfactor for your conditions: material, thickness and fabrication method/machine.
Instead of a fixed Kfactor, You can construct a bend chart with the correct values for different cases.
This way, you will have the correct Kfator for all your conditions.
To create a bend table, check this.
https://www.youtube.com/watch?v=_rffkLWT-jI
https://www.youtube.com/watch?v=HSzEJi386Ik&t=350s
CCarreiras
HI!
The standard factor in inventor (0.44) is an empiric standard starting value.
Despite the k factor selected, what really matters, is your final goal, and this is depending on several factors.
Different conditions (Fabrication processes, thicknesses, material, etc ), would give a different final result using the same flat pattern size extends.
The proper to achieve the correct kFactor is to do some real controlled samples: starting from a flat pattern calculated with the standard k factor and measuring the final result.
Based on these tests, it's possible to refine the proper Kfactor for your conditions: material, thickness and fabrication method/machine.
Instead of a fixed Kfactor, You can construct a bend chart with the correct values for different cases.
This way, you will have the correct Kfator for all your conditions.
To create a bend table, check this.
https://www.youtube.com/watch?v=_rffkLWT-jI
https://www.youtube.com/watch?v=HSzEJi386Ik&t=350s
CCarreiras
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
