CAD Forum

I believe I have a pretty good grasp of gauge tables, but now I'm wondering about bend tables. I have all the values tested for making a table but the implementation seems extremely convoluted and the SWX Help is pretty vague....

• Does a gauge table automatically reference a bend table?

• Do you use a separate bend table for every thickness and material?

• What happens if you use a bend table and need an angle that isn't available?

• Does SWX automatically know if the cell values are for K-factor or BA or BD?

• Can a bend table disagree with a gauge table that controls the same part (for default K-factor values)?

Is it just me or did Solidworks make this way more complicated than it needs to be?



Pinging..... @Dennis Bacon, @DennisD, @KevinC, @gupta9665.

@mike miller,
I ran the engineering department at place that did a ton of sheet metal. Though this is not explicitly answering your particular questions, it does address how we resolved the same issues.

We did a little homework and made some measurements and calculations. This allowed us to improve our part and flat pattern design to the extent we dramatically reduced our scrap and WIP, eliminated our bottleneck (Yes! Everyone in engineering/manufacturing should read The Goal at least every other year!), and were even able to design-in more features - all because we had good data and knowledge. Since we had our own sheet metal fabrication we were responsible for the flat patterns as well as the design of the finished parts.

Here is what we did:
1. Measured the actual thickness of our metals. Believe it or not, they were not in the middle of the published ranges for the gauges. We updated this every six months or if we got a different supplier. It is astounding how many people just use the nominal gauge value and expect accurate results. That might be okay for the part design for some (we weren't satisfied with that), but that will not work for generating accurate flat patterns.
2. We invested the time to do some bend studies. We took scraps of all the gauges and measured their thickness (again) and their lengths. Then we gave them 90 degree bends and measured the resulting legs.
3. We did step 2 for all gauges and for all press brake punch/die combinations.
We used a spreadsheet to calculate our K-factors for our combinations of tooling and thickness. You can go as detailed as you want with this, but we made separate tabs for each material and were careful to indicate the tooling. (We even looked at grain direction, but for us the typical difference in the K-factor was on the order of 0.02 so we determined that was not significant enough for us to worry about.)
4. We had about 15 people in our department so I made them all participate in the data collection and calculations. Some were understandably resistant to this until they saw with their own eyes that we could get accurate results! Then they became diligent in properly updating and applying the technique.

We were making multi-bend parts (typically 3-4 parallel bends in one direction and then more bends in other directions) in 12-gauge with only .002-.004" deviation from target. Most of our bends were 90 degree, but we did not encounter any errors with more open bends. This absolutely worked!

See the attached files for more explanation and an example spreadsheet.

I would say WAY more complicated than need be. Until our VAR explained it that there are N different methods to do this for all the various needs out there. We were new to SW and we had many irons in fire so I didn't have time to learn full detail of each method. Tech support spent a couple hours with me on the phone going over what type of sheet metal work we do and then determined the method to use. In the end we just have two excel files, one for steel and one for alum. We only use 2 k factors, one for steel and one for aluminum. It is not dependent on material thickness. For the rare cases where the tooling cannot produce the radius or causes a different stretch we edit the values in those specific features, not for the whole part and do not add options to the table for those.
Maybe there are benefits of the other methods, I don't know. I think the answer requires more details about the usage and needs specific to your situation.

@DennisD yes, we actually used your method to determine the K-factor for each material thickness we use. My biggest question now is how to implement this. For example, the gauge table will specify a K-factor across the board, but obviously that won't agree with a bend table...

Would you be so kind as to share a copy of your table so I can see how it's set up?

@bnemec, how accurate is your table? We have a different K-factor for every thickness of material so we can't just drive everything from a gauge table. Besides, some material may use two different sets of tooling depending on the required inside radius and angle.

mike miller wrote: ↑Mon May 17, 2021 4:23 pm @DennisD yes, we actually used your method to determine the K-factor for each material thickness we use. My biggest question now is how to implement this. For example, the gauge table will specify a K-factor across the board, but obviously that won't agree with a bend table...

Would you be so kind as to share a copy of your table so I can see how it's set up?

Once we had our K-factor spreadsheet we then made a part template for sheet metal that already had the spreadsheet included. This was in 2007 when we did this so the inclusion of the spreadsheet in the template was the easiest and most reliable method at the time. I haven't looked at linking the file. We would simply open the file and look up the thickness of the material and K-factor and then use those in the file. There are probably better ways now to to link to this information, but this worked for us.

You can use different K-factors for different bends within the same part.

As a Rule of Thumb we found that if the IBR was >= twice the thickness then a K-factor of .45 worked pretty well. But most of our bends were tighter than this and since we had hard data with our actual tooling we totally got rid of that "Rule of Thumb".

I don't have the K-factor spreadsheet from that company anymore. Sorry.

How accurate do you need?
For example:
0.125" material 0.1 k is 0.019" different in length on 90 deg bend.
Most shops are good with that.
Can you bend within that tolerance?

Simple K-factor apply to whole sheet all bends. Regardless of bend angle and rad.

Bend table can be customize for each bend angle and rad combination.
So first you'll need to do test for each you want to set. So you have data for the table.
If you're that picky, grain direction will make a different. Also hardness of that batch.

mike miller wrote: ↑Mon May 17, 2021 4:23 pm @bnemec, how accurate is your table? We have a different K-factor for every thickness of material so we can't just drive everything from a gauge table. Besides, some material may use two different sets of tooling depending on the required inside radius and angle.

Frankly, not very. We've gone through the process similar to what Dennis explained and found that there are so many continuously varying parameters that shooting for mean material behavior is the best route for us, at this time.

We have a mix of die run parts and laser and break parts, historically we do not alter the radii and k-values specific to one or the other. That may change some day. Even if just for break formed parts we might be able to dial it it, but the hardness and thickness of the material we get in varies so much I'm not convinced we would be better unless we revise the parts for every heat (which is not practical.)
Die run parts, the exact same coil is sometimes used for several parts (trying to help keep raw inventory moving) but we've seen that different tools make different bends in different stations of the progressive die, from the same coil. After that our flat patterns are not really used by the tool shops that do the progressive dies, it's their job to make a tool that produces the part per print given our "run of the mill" material properties.
In theory we could come up with a near perfect bend table for all our material but in the end we are better off designing the parts so that the significant features are measurable and able to be held and the next step (usually weld fixtures) position the part in such a way that makes good weldments.

A infinite circular rabbit hole.

@mike miller

There are the old gauge tables, they only contain thickness and available radii for those thicknesses. You have to use an accompanying bend table or manually enter K-factor or bend allowances.
Then there are the newer gauge tables introduced a few versions back that combine gauge and bend tables. These you can create several gauge thickness each with different "K-Factor" or "Bend Allowance" for different combinations of bend radii and angles.
With newer processes we have gravitated to the newer table. but as mentioned by others, you have to do a bit of trial and error to figure out the values for your equipment and process.

Thanks, @jcapriotti! Apparently the solution is to forget about Bend Tables completely and use the new Gauge Tables for everything. They control material thickness, material alias (gauge name, SKU #, or nickname), available radius, and K-factor all from one file. Eventually, I will create a separate table for each material and process, although 90% of our work is HRS bottoming.

From the interface, select the appropriate table, the material thickness, and radius (if there is more than one available). The Bend Allowance type will default to Gauge Table but this can be changed to reference a Bend Table or to key in a K-factor.
Attached is the HRS table I completed this morning. It is not complete yet but it should give a general grasp of how it works. Thanks to all who helped with this!

mike miller wrote: ↑Tue May 18, 2021 8:33 am Thanks, @jcapriotti! Apparently the solution is to forget about Bend Tables completely and use the new Gauge Tables for everything. They control material thickness, material alias (gauge name, SKU #, or nickname), available radius, and K-factor all from one file. Eventually, I will create a separate table for each material and process, although 90% of our work is HRS bottoming.

From the interface, select the appropriate table, the material thickness, and radius (if there is more than one available). The Bend Allowance type will default to Gauge Table but this can be changed to reference a Bend Table or to key in a K-factor.

2021-05-18 08_26_36.jpg

Attached is the HRS table I completed this morning. It is not complete yet but it should give a general grasp of how it works. Thanks to all who helped with this!

Michael,
Do you really have an option to bend .5" thick material with a .188 radius? Am I missing something?

DennisD wrote: ↑Tue May 18, 2021 8:50 am Michael,
Do you really have an option to bend .5" thick material with a .188 radius? Am I missing something?

With bottoming we can get close.....close enough for us, ennyhow. We don't do much 1/2" material, and it should probably be rechecked. At least the flat patterns are working...

EDIT: I just stepped out and checked a 1/2" part. Because of the punch nose radius, the inside part radius measures .188"; although there is a tiny bit of distortion happening inside the vee of the die. We normally oversize the clearance radius for a bracket fitting into a bend anyway, so it doesn't really matter in the long run.

mike miller wrote: ↑Tue May 18, 2021 9:14 am With bottoming we can get close.....close enough for us, ennyhow. We don't do much 1/2" material, and it should probably be rechecked. At least the flat patterns are working...

That is the key! All the suggestions are ideas on how to achieve that objective.

DennisD wrote: ↑Tue May 18, 2021 8:50 am Michael,
Do you really have an option to bend .5" thick material with a .188 radius? Am I missing something?

Bending along the grain, I'd be concerned the material would crack as that is pretty tight for that material thickness. For 0.5 plate we would usually try for a radius of 0.5 - 0.75 and tell the engineers to go as large as the design allows. If we do bend that tight, we usually have to specify to bend against the grain.

It's like others have mentioned, it all depends on the accuracy that you require. A generic k-factor of 0.4 to 0.5 may just do it for you if precision isn't paramount. We've done extensive in-house testing using different tooling (punch and die combinations), machinery, materials, to achieve what works best for us.

We use Gauge tables, one each for aluminum, stainless steel, and carbon steel. Which once are set incorporate the appropriate k-factor with the corresponding metal thickness.

The Fabricator.com website house a wealth of information when it comes to sheet metal techniques and fundamentals.
https://www.thefabricator.com/search?q= ... ndementals