.ipt bend part...flatten?

[Anonymous]

When you are making an .ipt and decide to bend the component and decide to use "bend part" tool, which is similar to what you would do in a sheet metal design. Is there a way to produce a flat pattern back out of this after you bend it. For example, when producing a shop drawing on an .idw. Any information would be great. You can do it with a sheet metal design, but not if you create a basic part file and do the bend part. Thanks in advance

Dan

[JDMather]

It is almost always better to model as folded using the sheetmetal tools. If starting from flat use the Fold rather than Bend.

In any case if modeled correctly you should be able to get a flat pattern. Even base solids from other CAD programs can generate a flat pattern. Zip and attach what you have so far.

[Anonymous]

This is a generalization of what needed done. One of my "less experienced" drafters did this and provoked an interesting question on how how to create a flat pattern from the "bend part" tool.

[Anonymous]

Dan,

The part bend feature does not take into account the material deformation
that happens in the bend zone - so: NO, you can't get an accurate flattened
state from your bent part (there is no command to flatten a bent part).

As JD suggests, can you model the part as sheet metal?

--
Gary R. Smith
Autodesk Manufacturing Solutions Division
Technical Publications - Subject Matter Expert
Portland, OR
2.33GHz 2GB IBM ThinkPad T60p; XP pro SP2
ATI Mobility FireGL V5250 driver: 8.293.1.0

[Anonymous]

OK, so the bend part tool, is mostly just for representational use only. It does not take into account the deformation in the material. The part in this situation can be made from a sheet metal stand point relatively easily. I just didn't know if there was a way to use bend part or not. Thanks for the info guys. Take care and have a good day Message was edited by: JerseyShoreDan

[JDMather]

>One of my "less experienced" drafters did this

I would start by having them read this document, Sketch1 was not constrained and no use of symmetry in the model.
http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

[JDMather]

Double click on Flat Pattern.

Don't use this one. Message was edited by: JD Mather

[Anonymous]

Does Autodesk have any intentions of making the 'bend part' command functional? This would be useful for designing bent tube, pipe, or roundbar. As of right now, it does not appear that Inventor is capable of handling designs that utilize these bent materials. We are evaluating the purchase of non-Autodesk software that will produce this, in order to determine cut lengths of these types of product.

Thanks,

Chad

[JDMather]

Bend Part works fine here.
What are you trying to do?

Is your real problem statement  to unfold a bent pipe?

What is this "non-Autodesk software" that will produce your geometry?
Attach example file from this non-Autodesk software.

[Anonymous]

Yes, the bend part feature allows you to bend a part, but the final outcome is not an accurate representation of a real life bend based on the base length. This is a dangerous design pratctice if Inventor cannot determine the correct part dimensions based on initial length.

Thanks,

Chad

[JDMather]

Post the example from other software.

Most model up the finished form and have the shop determine the initial blank length to get there.
Bend allowance will vary from machine to machine, even machines of the same make.

The finished bent part is what must pass inspection.

Correct part dimensions of finished part is the design intent - not initial length.

Bottom line - model in finished form - not flat to bent.  It would be nice if Inventor could then give you the starting length with reference to bend allowance.  It might be nice to unfold bend-by-bend for documentation.

In any case, post the "solution" from the other software.

[pauldoubet]

---

@Anonymous wrote:

Yes, the bend part feature allows you to bend a part, but the final outcome is not an accurate representation of a real life bend based on the base length. This is a dangerous design pratctice if Inventor cannot determine the correct part dimensions based on initial length.

Thanks,

Chad

---

Chad,

It is possible to create parts using the Bend Part command and have the developed length be accurate. It is not something that is as easy as the sheet metal flat pattern function. It is not that difficult to do either, it will depend on what your work consists of and if you want to have that function automated like it is in sheet metal. All that is required is to create a sketch plane for your bend line that is at the correct location to match the neutral axis of your bend.

As JD pointed out you need to supply all of the input based on your own machines and tooling, etc.

Hope this helps, Paul

[Anonymous]

Right, the design intent is the final bent part, but as you said, the shop must determine the initial cut length, if this is not supplied. Our manufacturing site uses a software called Bend-tech to determine these lengths. This process takes place in the drafting department so that the cut length can be called out on the print. Bend-tech seems to produce accurate information on all the various different types of materials and machines. I haven't purchased the software yet so unfortunately I can't send you any files but below is a link to their site:

http://www.2020softwaresolutions.com/products.htm

[JDMather]

That doesn't look too expensive.  If it works it should pay for itself on first job.

[Anonymous]

Those are my current intentions but I would love to see Autodesk provide this functionality to eliminate the need to have multiple instances of the same part. We link most of our part descriptions to parameters to maintain accurate descriptions. This way if a part length changes, the description will update with it. When a length parameter is not available, this must be updated manually, which opens the door for human error. We will probably proceed with the bend tech software.

Paul, I'm interested in what you mentioned about automating accurate part lengths, but I'm unclear on how to do that. Could you give more detail, ie. where to input machine specs and how to setup part files...

Thanks,

Chad

[pauldoubet]

If you would post a screen capture of a part like you fabricate I would create an example using the bend part. If that is not possible I can create a bent round or square tube based on my own experience and post the part here.

Paul

[Anonymous]

That would be great. I've attached a part file.

Thanks,

Chad

[JDMather]

I don't understand why anyone would use Bend Part for something like this anyhow?

It ends up with strange dimensions (and would be even more difficult with bend allowance).
Why not model "as bent" using Sweep command that would give exact finished dimensions with no calculations - no fudging?

[Anonymous]

Logically, when bending any part in the real world, you would start with a straight piece. You would then bend it to obtain the end product. If you were under the assumption that Inventor was able to compute bent parts, you might attempt to use it to do that. The previously attached item is a handle, the final dimensions of which were not as critical compared to the need for the flat length to actually match the end result.

Sweep or bend, Inventor doesn't give a flat length for this either way. It really doesn't matter why the user would want to do this, the real question would be, why does Inventor have a bend part command if it has no practical purpose.

[JDMather]

You have lost me.
The software you linked creates the bent tube the same way Inventor does.
The only difference is (I haven't verified this yet) is that it then gives you the starting cut length calculation.
The ideal technique is to model in finished form any way you look at it.  I would always always always model something like this in the finished form.  It would be nice for Inventor to then calculate the starting length.

Bend part should very seldom be used.  There is almost always a better way.

One logic use might be to bend a helical spring which would be very difficult to do using any other technique.