Hi all,
I am having a lot of trouble folding a 45 degree bend (See attached Detail Drawing, Parts and Bend table). I am using a bend table and I cant get close to the dimension of the brake press bend sizes without a error ocurring in the mitre flange.
If someone could take alook at the 3 attached documents and tell me where I am going wrong that would be appriciated.
Good morning Jeremy,
Take a look at the attached documents, Did you have a chance to bend up samples?? I always rely on the SW generated sheet metal, however a high precision bending shop would need to make a few changes in the bend allowances and bend radius table. There is a difference if you have the manufacturing in house, then the guys on the floor need correct dimensions, however if you send the part out to get folded then all you need is overall part dimensions, as the dies and punches and machine may bend a little different.
I add a note in the PDF,
Later,
John
Good morning Jeremy,
To give an accurate answer I would need to see a formed view that would show me what your dimensional intent is for your parts. In other words, I need to see what your actual part dimensions need to be.
In the flat Solidworks is showing the positions of the bend centerlines for your brake operator, those are calculated from your bend table as shown here. Looking at your bend table I see the bend deduction is larger for the 45 degree bend than the 135 degree bend, that appears to be incorrect. If you're using an Amada press brake I can understand how these two were inverted.
To an Amada control, a 90 degree bend is 90 degrees. While a 45 degree bend is entered on the control as 135, or 180-45. A 45 degree bend is 180-45=135 degrees.
I would suggest using .42 as a K factor for all bends except for the 90 degree, I would assume you know what your actual deduction is for a 90. I remodeled your part using a .42 K factor and the flat results are shown below.
Hi John,
All folding is in house we have a press brake. I have folded up samples and the exact measurements are noted on the detail drawing, Material thickness is 2mm. I also have folded a test peice with the solidoworks dimension and the Overall is now 25mm thick.
Bernie I used your .42 K-Factor and it worked perfectly, Is there a table of K factors i can use for material thickness 1.2mm and 1.5mm Stainless Steel? or is it trail and error?
Jeremy,
You can develop your own table based on real world testing on your equipment and tooling.
Create square blanks of material and test bend. Then you can calculate the bend deductions and log in a chart.
http://www.ciri.org.nz/bendworks/
BendWorks has a nice pdf explaining the process. He also has a program called BendWorks that is handy for this type of task.
Cheers,
Anna
Jeremy,
I'm glad it worked out. I'm not really a K factor guy, I use real bend deductions and allowances that have been tested and committed to writing. That way if you have three guys doing programming you'll get consistent results no matter who does it. If you have an issue with a job could you ask your press brake guy if he got a .42 or a .50 K factor on that bend? Every print I issue for the floor has the bend radius and the bend deduction I used to calculate the flat and for each bend if they are not similar.
That allows the press brake guy to check as he goes along. For instance, put one bend in and check to see that he achieved the bend deduction by measuring before and after the bend. Maybe it's too much for what appears to be counters that you're making. Not an insult, please don't take it as one and I may very well be wrong about that. My favorite saying is, it can't come out right if it doesn't start out right.
I have a spreadsheet that helps me calculate bends other than 90's. Actually the spreadsheet doesn't really work for 90's either. There still is a judgement call, at least to me. If you're bending using dies that are open 4 times the material thickness plus 1.42 times the radius you should use a K factor around .40. If your using dies about 8 times plus the 1.42 times the radius open you should be using .50.If you coin with sharp tooling, maybe .33. The 1.42 I used relates to a 90 degree bend. In 40 years of precision sheet metal I've never seen a K factor less than .33 or greater than .50. Some progressive tooling could generate a K factor in the range of .3. That is probably due to the 'wiper style' of tooling but I don't have the experience to comment on that.
Then again all that can only be verified if you can really and accurately check the results. I don't have the drawing in front of me as I write this but did you have the tooling for the two bend radius on the part? Was it 1 and 2mm? Do you have the acute angle die for the .2mm radius on the 135 degree overbend? Without knowing all those things I can't really say how to get better but to get a real understanding of how the parts will be bent and use that information to design the parts in SW. You'll get infinitely better results and if you follow it religiously you'll also get better results from the floor.
I see Anna Wood just posted about Bendworks. It does have some advantages over my spreadsheet and definitely deserves to be on your PC.
Good luck!
Good morning Jeremy,
To give an accurate answer I would need to see a formed view that would show me what your dimensional intent is for your parts. In other words, I need to see what your actual part dimensions need to be.
In the flat Solidworks is showing the positions of the bend centerlines for your brake operator, those are calculated from your bend table as shown here. Looking at your bend table I see the bend deduction is larger for the 45 degree bend than the 135 degree bend, that appears to be incorrect. If you're using an Amada press brake I can understand how these two were inverted.
To an Amada control, a 90 degree bend is 90 degrees. While a 45 degree bend is entered on the control as 135, or 180-45. A 45 degree bend is 180-45=135 degrees.
I would suggest using .42 as a K factor for all bends except for the 90 degree, I would assume you know what your actual deduction is for a 90. I remodeled your part using a .42 K factor and the flat results are shown below.