Sheet Metal: Bend Radius+Unfold Table

[bmeraz]

Hello,

My employer requested I add our sheet metal suppliers bend tables to inventor to expidate release of flat patters.

My intention is to create sheet metal styles specific for this supplier so that our users can select that supplier if we are designing parts to go to them.

After reviweing the bend tables the supplier has provided I have come to the following conclusion:

1) They have only provided a bend table for 90 degree bends

2) For all other bends I am to use the Kfactor provided in the table

In terms of Inventor I understand the following:

1)I need to copy the default unfold style 

2) Change from linear equation with kfactor to table driven

3) Edit table to include material thickness the Bend Radii and the angle and the Bend Deduction

4) Input the backup k factor to the one provided by the manfacturer

And this is where it gets funky.

When I unfold a part with the above values I get the following message: 

Create Flat Pattern: problems encountered while executing this command.
Part2: Warnings occurred during update
Part2 (Flat Pattern): Warnings occurred during update
Definition1: Problems occurred while building this FlatPattern
Error querying the Bend Table. The angle or radius are outside the table boundaries. The input values were: Thickness: [0.064000], Angle: [90.000000], Inner Radius [0.064000].
Error querying the Bend Table. The angle or radius are outside the table boundaries. The input values were: Thickness: [0.064000], Angle: [90.000000], Inner Radius [0.064000].
Error querying the Bend Table. The angle or radius are outside the table boundaries. The input values were: Thickness: [0.064000], Angle: [90.000000], Inner Radius [0.064000].
Error querying the Bend Table. The angle or radius are outside the table boundaries. The input values were: Thickness: [0.064000], Angle: [90.000000], Inner Radius [0.064000].

After many headaches and learning about bending etc (the foleys of google search) I came to the conclusion that the default bend radius is preset for material thickness. As a result the bend radius in the bent portions of the part are too large to coincide with the bend radius I entered into the bend table. 

Pause: Thank you for your patience on this long post....

So it seems I need to do the following:

1) Set up a rule that tells inventor that when using this specific sheet metal style to use the material thickness for all bend angles that are not 90degress

2) For all other bends to use the radius from the provided bend table

3) Edit the a custom unfold rule to include the kfactor, bend radius, bend angle, and thickness of the material.

My questions are as follows:

1) Am I understanding the workflow as to how to edit the bend table?

2) Am I understanding what the issues is when I unfold the part and get the above error?

3) The solution I proposed (about different bend radius depending on the angle) does it make sense? And if so how would I go about implementing that?

For your reference I have provided the bend table given to me and the sample part I am working with.

Any and all help is much appreciated.

Thank you,

Baudelio

[innovatenate]

A sheet metal styles only uses one global/default unfold rule when calculating the flat pattern. You must pick between:

• Linear (K-Factor)
• Bend Table
• Custom Equation. 

You may override an unfold rule for a specific feature (e.g. flange).

Bend Tables and Custom Equations are the only available methods that will change the allowance/deduction based upon angle, radii, and thickness for a provided material. From the posted error messages, it sounds like you are attempting to flatten a part with a bend table selected as the unfold rule. However, the exisiting bend angle/radii are not defined in the table.

Since the Bend Table only appears to include the allowance and deduction at a single angle (90 degrees?), I would just insure that the k-factor is set to match the the table. Tips on how to backward calculate the K-Factor:

http://www.widom-assoc.com/AU-MA31-2.pdf

If the supplier can provide further information about they would calculate the allowance/deduction with respect to bend angle, and bend radius, then you may use a bend table or a custom equation unfold rule to insure that your flat patterns will be "correct." If they cannot provide this information, then your flat patterns will never be "correct" since thickness, angle, and radius will effect the allowance/deduction. I've heard some press brakes will even record a material's heat number and make adjustments, since one batch of material may differ from another from the same supplier. 

Consider whether providing prints of flattened patterns or only the fully-dimensioned, formed parts to the metal forming supplier is the best practice. Most sheet metal suppliers should have the capacity to  work out the details of how a part is made.

I hope this helps. Let me know if I may clarify anything.

Thanks,

[bmeraz]

Nathan,

Thanks for the quick reply.

My apologies I havent been able to respond myself I have been bogged down with some other issues.

After reading your reply I think I understand what you are telling me.

However I think that maybe you misunderstood me a bit also.

The sheet metal supplier is only providing bend allowance/deduction values for a 90 degree bend you are correct in saying that.

However note that the bend radii is given for a 90 degree bend. This is shown in the third column.

My understanding of this is that the value provided in this column is the bend radius of that gauge for 90 degrees.

So what I do is go into the Bend table editor and input the values listed (see attached image)

I get the error message when the bend radius of the part is at material thickness if i manually adjust the bend radius this table now works and the part unfolds.

Perhaps the issue is that I dont understand the difference between bend radii listed in the unfold bend table and the bend radius listed in the bend radius defaults...

Is there ever a moment in which the bend radius for flange matches the bend radii given in the unfold table? It seems that you cant bend a part with a default value if the radius is determined by the ability of the air press. I hope that make sense?

After discussing this with the supplier they asked that all I do is:

• Use bend table and the given bend radius in that table for 90 degree flanges
• Use the provided k factor and material thickness as bend radius for all non 90 degree flanges

The question becomes... how do I tell inventor to use material thickness for all non 90 degree bend and to substitue a value for a 90 degree bend??

Or am I just supposed to adjust the bend radius manually for all 90 degree bends?

[innovatenate]

Baudelio,

Thanks for the update.

I interpreted column 3 differently in the first table (X-Manf_Bend_Table.png). The column 3 header is "Available Bend Radius," which sounds synonymous with Minimum Allowable Bend Radius. If I'm remember correctly, there is a rule of thumb that states that the Minimum Bend Radius for any thickness is approximately equal to the materials thickness. There are exceptions to this rule, but this rule of thumb helps when designing parts in general. For example, in the below table a gauge 4 sheet may have a bend with the developed radius equal to .1880 or .greater (provided the supplier has the correct die available). A bend radius smaller than .1880 may result in cracks on the outer radius of the part.

There are some sample Bend Tables as a .txt file in the Inventor Help and in a default location. You should create or edit your own text file similar to the version in the below link:

Unfold Table TXT Sample.

.... OR... you may use the .xls or .txt bend tables files found in the following default location:

C:\Users\Public\Documents\Autodesk\Inventor 2014\Design Data\Bend Tables

If you review C:\Users\Public\Documents\Autodesk\Inventor 2014\Design Data\Bend Tables\Bend Table (in).xls., you'll note that there are two thicknesses contained in the same file, .060 and .120 (in). For Each thickness, there is a range of bend angles AND a range of bend radius.

You can then use the Import function in the Styles and Standards Editor to import an Unfold Bend Table Rule via .txt. file. see the link below for more information.

How to Import

After importing the text file to create a new unfold style, you'll see the following:

I hope this clarifies how a bend table can provide a custom deduction value for each thickness, angle, and bend radius, fully customizing the sheet metal unfold style inside of Inventor.

For the scenario you are inquiring about below regarding 90 degrees versus all other bends, you are right that you will need to manually control this. It may help to setup an unfold table. As you've seen, if a scenario outside the table is encountered, a warning should appear to let you know about it. Let me know if this helps or if you have any further questions.

Thanks,

[bmeraz]

Nathan,

Thanks for the clarification.

Fortunately my custom bend table will be significantly more simple.

Ill check out those files you referenced.

One more question... My interpretation of Back up k factor in the custom bend table is that it is used when no available value is in the bend table... i.e. non 90 degree bends. Is my interpretation correct?

Thanks again.

[mcgyvr]

I always recommend to NEVER give a flat pattern to an outside sheet metal vendor. That is just asking for problems.

Its a sheet metal vendors JOB to calculate the flat patterns to produce parts to your dimensioned prints showing the part in the "as formed" state. 

Any vendor that requests a flat pattern is NOT a vendor I would use. Heck ours are even constantly adjusting their press brakes,etc.. due to minor thickness variations in raw materials.. 

What happens when you change vendors..maybe because of a purchasing/cost/leadtime issue? Now your department needs to spend more time to recalculate/provide flat patterns for this new vendors tooling.. If you didn't provide flat patterns you or anyone at your company can simply have them quoted and produced to the formed print without having to add more internal time to a part.. The formed parts never change.. Flat patterns do..

IMO flat patterns/bend tables/kfactors are for companies that produce parts internally.. and should NOT be used with companies that source parts from outside vendors.. 

[jletcher]

I have to agree with McGyvr on the issue but I have clients that don't feel the same..

 All you need is the 90° kfactor Inventor will figure out the none 90° with that kfactor..

 I have 2 clients using ilogic to pick the bender vendor when they go to make the flat pattern it will ask to pick the bender vendor from a pick list. and change the kfactor..  Took time to set up but works...

 I have one client that set it up so it would work with all bender vendors but he does not have tight tolerance so he can get away with it.