Bend vs Fold

[farrous13]

Hello,

 

I know it might be a silly question.

 

But what is the difference between fold and bend?

 

I use fold most of the time. The bend option doesnt seem to work whenever i use it.

 

Thank you in advance

[Hopinc]

Yes, I can answer this one.

 

"Bend" is used to create a bend between two sheet metal faces that are unconnected, whereas fold operates on a sketch line on a single part.

 

If you click on the Bend command and then the question mark at the bottom left it will take you an explanation. Click Procedure at the top of the page and then select "Create a sheet metal bend," and finally the "Show Me how to create a bend" animated sequence.

 

In the attached images "fold" was used to on the left hand part, and "bend" between the two surfaces.

 

Regards.

 

Dave

[JD Mather]

........ and if you really meant - what is the difference between Bend Part in the modeling environment and Fold in the sheet metal environment, the Fold command take into account bend allowance in flat pattern (inside radius compresses, outside radius stretches).

 

I can tell you that I very very very rarely use Fold in sheet metal - users almost always use it incorrectly, in most cases there is a better technique than Fold.

[Hopinc]

Quote: " users almost always use it incorrectly, in most cases there is a better technique than Fold"

 

What are you saying they are doing wrong?

 

Dave

[JD Mather]

Quote: " users almost always use it incorrectly, in most cases there is a better technique than Fold"

 

What are you saying they are doing wrong?

 

Dave

 

Folding from flat rather than modeling "as folded" using Contoured Flange instead. There are some cases where Fold is only way - or best way, but in most cases Contoured Flange or other "as folded" sheet metal tools are much faster.

And modeling "as folded" you can easily model to desired end dimensions and not worry about bend allowance. Inventor will calculate that for the flat when you create Flat Pattern.

[sodapop808]

So what is the best way to make tapered flanges? I have been trying to do that for a complex panel shape and am pulling my hair out. When I create the panel as a model then shell it, I get errors and cant get it to work. When I create it as a sheetmetal part, I can't make tapered flanges. I recently started using inventor after many, many years of autocad and recently starting a job in the sheet metal industry so I am still an inventor newbie. I am using Inventor 2008.

[Hopinc]

Hi,

 

If I am understanding your question correctly, it is a relatively simple matter to make a tapered flange. At least it is 2010 and 2011. Sorry, but I don't have 2008 so I don't know if it is any different in this respect.

 

Presuming 2008 has the same sheet metal facilities, all you have to do is sketch a line on the panel surface corresponding to where you want your tapered flange to be (see the example in image 1) and then select "fold" from the sheet metal menu.

 

Next pick the line, and the pop down menu that appears will give you options such as angle, direction, inside, outside or centre of bend and bend radius. Image 2 shows the result.

 

If this is not what you want please attach a sketch of the shape you are trying to make.

 

Regards,

 

Dave

Edited December 3, 2010 by Hopinc

[sodapop808]

You are tapering the flange so that the legs are 90 Degrees to the end of the flange. I need the legs perpendicular to the face. Any thoughts?

[JD Mather]

When I create the panel as a model then shell it, I get errors and cant get it to work. ..

 

I've been watching your threads with interest - but it is kind of hard to say how to model it if you can't model it. (does that make sense)

Compounding the problem is you are using 2008.

 

Post the part as close as you can get it using the standard modeling tools (don't need to shell - I can figure that out).

 

I can tell you my solution is extreemly unlikely to include a Fold.

[sodapop808]

I am now on 2011. I have tried a couple of different ways of getting to the end result, all of which I have failed at. I have started with a primitive solid, then used shell, then ripped corner seams, then try adding bends and the part fails at the face break.

 

I have tried using sheet metal environment, and I get the face to break properly by using lofted flange, but can't add a flange that returns 90 degrees while the sides are parrallel with the corners.

 

I am sure that I have tried to run before I could walk, but I guess that how I roll.

 

I will attach 3 files. One is the primitive solid shape (Faceted AL Primitive.ipt), one is the extent of my sheet metal attempt which is the closest I have come(Faceted AL 02.ipt), and one is my shell attempt (Faceted AL From Shell).

AL Panels.zip

[Hopinc]

Hello sodapop808,

 

Please find attached herewith a solution to your problem. I tried to convert from a solid to sheet metal without success, but the answer was a combination of both part modelling and sheet metal. It worked just fine without any problems whatsoever. I had anticipated a struggle, but in the end it didn't take long at all. Sometimes you just have to think outside of the box.

 

Regards,

 

Dave

DRH_solution.zip

Edited December 12, 2010 by Hopinc

[sodapop808]

A very talented effort indeed! However, because some of the sketches are unconstrained, the model seems to have problems when I try to update any of the dimensions via Parameters Manager. This part will be variable in both height and width as well as the "tall" corner and "short" corners. I too was able to get close to your results this way. Your corners,however, are definetly steering me in the right direction. I will try to work with your model to see if I can constrain it and make it update. Thanks for your input!!

[Hopinc]

Hi sodapop808,

 

You are welcome. I am glad I could be of help.

 

Regards,

 

Dave

Edited December 13, 2010 by Hopinc

[sodapop808]

So, this part only really works as an uneditable part. Anybody have a suggestion as to how to make it a Formula driven sheet metal part? Please also see my other post on this subject. I am really having a hard time putting into words how frustrating this is. If this is a hard part to make, please tell me so I know I am not going crazy! It seems as though it should be easy, but its not!

[JD Mather]

If this is a hard part to make, please tell me so I know I am not going crazy! It seems as though it should be easy, but its not!

 

Actually it is pretty easy. I put together a quick example that I want to tweak a bit before posting, but it is not a difficult part. I think my solution will be somewhat unique compared to other solutions you might get.

[sodapop808]

That would be so helpful!!

 

I am able to get most of this model working, but always seem to get down to one flange that is giving me grief. I was able to draw the flat pattern in autocad in a matter of minutes (OK maybe a little longer) as this is how I am used to doing flat patterns. However, with Inventor as one of our tools that is not being utilized, I am trying to convert over to Inventor. I am looking forward to any insight and am very appreciative of any lessons that you can teach.

[JD Mather]

I guess the hard part I'm having trouble understanding is you attached 3 different files that don't seem to be heading in the same direction.

Here is what I seem to gather is sort of common geometry between the 3 files.

This portion was relatively trivial - you will have to continue on with the geometry (pull down the EOP marker in the browser) for additional suggestions I might be able to provide on finishing the part.

This example was done in edu version - so delete after examining the technique.

I think you will find it significantly easier than the previous solution that was attached here.

Tray-jd.zip

[Hopinc]

Nice One, JD!

 

I had tried that method myself. It did not work for me because I did not delete the corner surfaces, and the corners would not work out. That is a good trick I will remember that.

 

Regards,

 

Dave

[sodapop808]

OK. Wow. I can't beleive how overly complicated my model was compared to yours! OK. You filleted the corners first. I'll make note of that. I have never tried it that way. I shelled it, then tried to rip corners and make bends. Then you did a delete face and thicken instead of a shell. Is there a reason for this? I would have never thought that way. I am going to try and do a model myself this way now. Thank you very much for such an elegant solution. Although you think it a simple part (and yours is!), I think it is because you are a Jedi master, and the solution was there from the beginning.

[sodapop808]

....but wait!! Your part can only be square. I need it to be able to drive the 24" dimension on both the width AND the height to any number I need from parameters... I will try a new model with the things I have learned and see if it gets me anywhere.