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Sheet metal + cross bend

Anonymous

Sheet metal + cross bend

Anonymous
Not applicable

Hello,

can enyone tell me if it is there is a command "cross bend" (like in solid works) in the sheet metal environment please?
Thank you.

 

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S_May
Mentor
Mentor

@Anonymous 

 

bitte ein Muster hochladen

 

Translation - Please upload a sample

JDMather
Consultant
Consultant

JDMather_0-1607089224488.png

JDMather_1-1607089268896.png

https://help.autodesk.com/view/INVNTOR/2021/ENU/?guid=GUID-F14FE540-6E64-4A4D-A813-D4C2A8DA5865

 

 


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


Anonymous
Not applicable

Thank you for the hint, but I 

already saw this in the forum.
I want to be able to create these croo bends in the folded environment (eg. a roof, see attached), so tha I can see the final form.

 

thank you

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JDMather
Consultant
Consultant

Attach your *.sldprt file here and I will create the geometry in Inventor.

If you no longer have access to SolidWorks, then get it as close as you can in Inventor and Attach your *.ipt file here.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


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Anonymous
Not applicable
Hello,
 
thank you for your reply.
In attachement you will find my sheet metal part.

I want to lift the cross bends (approximately 10 cm) upwards in the folded model.
 
Thank you.

cadman777
Advisor
Advisor

My older version of Inventor (2010) doesn't have any CrossBreak command.

Apparently the newer versions don't have it eitehr.

 

This is what comes to mind:

 

1. When doing platework, I would do this the hard way (manually) by using wireframe geometry with a slit along one of the breaks (to be welded), b/c the fab shops around here don't have the presses to make true true cross-breaks in plates. It's a lotta work to create this.

 

2. If the shop DID have the capability to make true CrossBreaks, then I probably would make an iFeature and use that in the model. It's a bit tricky, b/c of the variety of edge conditions this feature would need to accommodate. I'm going to try to do it and see if it's possible. I abandoned iFeatures many years ago b/c unless they're real simple and use the most basic features, they fail on me every time. Maybe I just don't know how to make complex iFeatures?

 

3. Also, to make a true CrossBreak you can do it the hard way and make the feature first, and make the sheetmetal flanges afterwards. See two attached examples.

 

4. I noticed that the SW sheetmetal CrossBreak feature is not really a true cross-Break. This can be done in Inventor using iLogic and some VBA programming. Or it can be done manually like JD shows, using Inventor's CosmeticBendLine tool in the sheetmetal flatpattern module. But these only work in the flatpattern, so you'll have to make another sketch in the folded part module to get the appearance of a CrossBreak on the folded model in your drawing. You have to 'Include Sketches' in the drawing to see those sketch lines. They don't work in the ISO views in my version of Inventor. Don't know if that's fixed in newer versions.

 

Here's a quick tutorial on iFeatures, in case you've never used them:

https://www.youtube.com/watch?v=Lu1sr_Ol720

 

... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator

IgorMir
Mentor
Mentor

Hi Steve,

You are saying - you want a crease of 100mm. Well, that is technically - a stamped part. Not a true sheet metal part.

Initially I thought you need the elevation of the crease of 10mm. That's different. It can be done by utilizing two parts in the design. Part1 is what you put in your assembly. Part1 drives Part2 via linked parameters. Part2 is for extracting a Flat Profile. It will work since the crease itself doesn't stretch the material that much. On a panel that size you can go to 20 mm, I think. That would be better to discuss with the workshop people. 

Part3 represent a sheet metal part with the pyramid apex of 100mm. While it seems to work - I would be hesitant to go this way. All parts are in IV2020 format.

Cheers,

Igor.

 


@Anonymous wrote:
Hello,
 
thank you for your reply.
In attachement you will find my sheet metal part.

I want to lift the cross bends (approximately 10 cm) upwards in the folded model.
 
Thank you.

Web: www.meqc.com.au
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cadman777
Advisor
Advisor

Find attached an example of an iFeature for your roof. The problems with it are, I couldn't get the fillets to work on my older version of Inventor, so I moved the EOP marker up above the fillets and then made the iFeature. But maybe you can try making your own iFeature with it? I'm pretty sure I did it right. Also, the wall thickness isn't right. I tried like crazy to get it to work, but couldn't. Don't know if newer versions of Inventor can make this? I can't see Igor's parts, so not sure what he did.

 

Find attached 2 files:

1. the Template (for making the iFeature), and

2. the iFeature on a simple sheetmetal part w/flanges (sort of like you show in your pic).

 

This is not elaborate, and I kept it simple, b/c the more complex you make it, the harder it is to predict its reliability when in use. This took me a number of tries b/c the dang fillets kept not working. After you use the Template to make your own iFeature, when you're done placing it on a sheetmetal face, make sure to add the fillet on the concave leading edge (= Thickness*2) to complete the iFeature.

Note: I learned how to make these using TEDCF's tutorials. They are excellent!

... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator

IgorMir
Mentor
Mentor

Hi Chris,

It is not an issue to create such a shape. The quest was to make it as a sheet metal part. Or so I understood anyway.

Here are two screen shots to show how the part I made looks like.

Cheers,

Igor.

Web: www.meqc.com.au

cadman777
Advisor
Advisor

Very nice Igor!

Perfect flatpattern.

I'm going to try it your way tomorrow.

The reason I wanted to do it with a 'boss' is b/c of what this guy does in this SW video:

https://www.youtube.com/watch?v=lXevCDV0D1c

(start @ the 13:10 minute mark)

I've seen this done but never really had occasion over the years to do it myself.

The fabricator needs a press-punch machine to do it, and nobody I know has that capability.

Cheers...

... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
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cadman777
Advisor
Advisor
Accepted solution

Hey Igor,

I like the Lofted Flange command!

Never used it before.

It's much better than the way I did my first one.

Anyway, find attached my version of it the way I usually do things.

This part will break if the Apex is too high with relation to the Length & Width.

Don't know the OP's dimensions, but things looked proportional enough to work like the attached.

... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator

IgorMir
Mentor
Mentor

Hi Chris;

Thanks for sharing, much appreciated. I hope - Steve will find it useful too. 🙂
Cheers!

Igor.

Web: www.meqc.com.au

Anonymous
Not applicable

Hello everybody,

 

thank you all for your awsome input.
part crossbreak1c is the one that does it for me!

 

I needed a real sheet metal part that could be folded and flattened.

 

Thanks again!!!

 

Steve

cadman777
Advisor
Advisor

Hey Guys,

 

Took me 2 days of fiddling around with this between other stuff, but I think I've finally got a CrossBreak iFeature that'll work. Check out the attached.

 

I have to give the credit to TEDCF lessons on Advance iFeatures and Punches for sheetmetal. Without those lessons, I'd be SOL on this one. This gives me hope for other things I've been wanting to do for some time now! Anyways, if I had more time I'd make it an iLogic-driven part with a UI and limits the Parameters so the thing won't break if the dimensions get too crazy. It'll break if you use extreme numbers for Length/Width, Height and Thickness. So keep things proportional and it'll work. The way it is now, the CB OALs are linked to the sheetmetal part's OALs so it updates more reliably.

 

Also, there's an underlying sketch to constrain the iFeature to the part. The 2 WorkPoints are necessary b/c the iFeature kept breaking without them b/c of the sketch failing to update after changing the Parameters (resizing). Also note the fillet added to the bottom inside perimeter, which is not part of the iFeature. The iFeature wouldn't work if I tried adding that fillet to the iFeature itself (Thanx Dave @ TEDCF!).

 

So you have a flanged sheetmetal rectangle base, a couple of locating WorkPoints, the CrossBreak iFeature, and a finishing fillet.

 

Hope someone gets some use out of this.

It was quite a challenge but a lotta fun!

Cheers...

... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator

Liam_Cooper
Explorer
Explorer
This crossbreak iFeature has helped massively that you have created. Thankyou.

gilbert_vasquez
Community Visitor
Community Visitor

Hello there,

Unfortunately, Inventor has "once again" fallen short.

Solid Works is a much better platform in Sheet Metal alone; not to mention so many other tools.

Much like you, I'm in urgent need to use the "Cross Break" in Sheet metal.

 

Best,

 

G. Vasquez

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johnsonshiue
Community Manager
Community Manager

Hi Gilbert,

 

Many thanks for your comments! Did you take a look at the alternative workflows mentioned above (Cosmetic Centerlines and Lofted Flange)? Did neither help create the desirable shape?

Thanks again!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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gilbert_vasquez
Community Visitor
Community Visitor
Hello Jonshon,

I thank you much for responding to my rant. 🙁

Here is the desired geometry:
[cid:a330b568-a47b-4562-86df-52cb19599dcc]

I have tried all the tricks to be tried and no luck.

Sad thing is, I was to created it fairly quick in Solidworks.

What's wrong with Inventor?
Is my question.
Here is a software I began using more than 20 years ago and it's nearly impossible to do something so simple.

I really have to do this for a Sheet metal shop like ASAP w/ a "Flat Pattern" so they can cut this part.

I'm trying to dream other options buuuuuuuuuuuut.............

Wheel C.

Thanks again amigo.

Kindest regards,


G. Vasquez
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johnsonshiue
Community Manager
Community Manager

Hi Gilbert,

 

Could you attach the image again? It was not attached last time.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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