Help! cannot fold & refold cone part.

[jefke1988]

Hi,

I'm struggling to make a good cone part.. I tried alot but cannot seem to get it right.

When i try to unfold/refold it the result isn't quite what i expected.

image before unfold/refold

image after unfold/refold

I have attached a part to illustrate the problem.

What do I do wrong?

Also see the iLogic form these parameters are variable.

[JDMather]

I would use some other technique that Unfold.

What is your next feature? (why do you need to Unfold?)

[wilkhui]

Hi Jef,

Sorry about this, you're not doing anything wrong.

I have good news and bad news...we're already aware of this problem and a fix is in the pipelines (pending validation etc). Unfortunately that's unlikely to be fixed in Inventor 2013, where this part was made.

I don't have a workaround for this weird behaviour but I'll keep trying, if anyone else reading this knows of one then feel free to chime in.

Cheers,

Indy

[jefke1988]

Hmm, maybe I forgot a part in my original post.

The cone is a "roof" with connections on it. But when the "roof" is large it is made out of multiple plates welded together.

To ensure a connection is not placed on a weld I wanted to mark the plate nesting on my cone (rather than build a cone out of multiple plates).

So I unfold my cone, so i can sketch my plates on it.

Refold the cone to place my connections.

[JDMather]

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@jefke1988 wrote:

...

So I unfold my cone, so i can sketch my plates on it.

Refold the cone to place my connections.

---

Now that I know the design intent - I can create a work-around for you.

Because you are using an earlier version - I will only be able to explain in pictures - and I don't have time to create the pictures right now, so check back later.

But what I will do is create a sacrificial planar face tangent to your cone and then use Project Flat Pattern and Cut Across Bend.

[jefke1988]

Now that I know the design intent - I can create a work-around for you.

Because you are using an earlier version - I will only be able to explain in pictures - and I don't have time to create the pictures right now, so check back later.

 

But what I will do is create a sacrificial planar face tangent to your cone and then use Project Flat Pattern and Cut Across Bend.

Please mark this response as "Accept as Solution" if it answers your question.

 Ok thanks!!

Hi Jef,

 

Sorry about this, you're not doing anything wrong.

 

I have good news and bad news...we're already aware of this problem and a fix is in the pipelines (pending validation etc). Unfortunately that's unlikely to be fixed in Inventor 2013, where this part was made.

 

I don't have a workaround for this weird behaviour but I'll keep trying, if anyone else reading this knows of one then feel free to chime in.

 

Cheers,

Indy

 And in what version would this be possible than? It's an important part of my product so i'm very interested in this.

[Mario428]

Just an opinion but you are doing it wrong?

Same old draw a part as a solid part and then wonder why converting it to sheet metal does not work.

See attached example of how I do a cone, it is a 1/3 section but you will get the idea.

[jefke1988]

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@Mario428 wrote:

Just an opinion but you are doing it wrong?

Same old draw a part as a solid part and then wonder why converting it to sheet metal does not work.

See attached example of how I do a cone, it is a 1/3 section but you will get the idea.

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I can't open the part. It's higher then IV 2013??

[blair]

Here's a technique that might work.

[jefke1988]

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@Blair wrote:

Here's a technique that might work.

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Yes, but creating the flat pattern isn't the problem. (if the roof is shaped like in the .pdf this is correct to get the shape as flat pattern.)

But i can't get holes made into my roof on the flat-pattern this way?

For now i'm sketching my plate nesting in 2D on my flatpattern but it's no ideal for placing the connections; or changing it's position.

[Mario428]

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@jefke1988 wrote:

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@Mario428 wrote:

Just an opinion but you are doing it wrong?

Same old draw a part as a solid part and then wonder why converting it to sheet metal does not work.

See attached example of how I do a cone, it is a 1/3 section but you will get the idea.

---

I can't open the part. It's higher then IV 2013??

---

I do cones using the Lofted Flange method, work plane at the desired height of the cone

One diameter at 359.9 degrees on main plane and the other also at 359.9 degrees on the plane just made. Use a lofted flange to connect them, in 2014 it flattens fine and returns

Be warned though that a hole normal to your planes will not be the correct shape on the flat pattern.

[jefke1988]

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@Mario428 wrote:

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@jefke1988 wrote:

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@Mario428 wrote:

Just an opinion but you are doing it wrong?

Same old draw a part as a solid part and then wonder why converting it to sheet metal does not work.

See attached example of how I do a cone, it is a 1/3 section but you will get the idea.

---

I can't open the part. It's higher then IV 2013??

---

I do cones using the Lofted Flange method, work plane at the desired height of the cone

One diameter at 359.9 degrees on main plane and the other also at 359.9 degrees on the plane just made. Use a lofted flange to connect them, in 2014 it flattens fine and returns

Be warned though that a hole normal to your planes will not be the correct shape on the flat pattern.

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So you say it can Un-fold & Re-fold just fine?

I have no problem creating a flat-pattern of the part, just Unfolding & Refolding it.

I will give it a go anyways.

[Mario428]

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@jefke1988 wrote:

So you say it can Un-fold & Re-fold just fine?

I have no problem creating a flat-pattern of the part, just Unfolding & Refolding it.

I will give it a go anyways.

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No fold & unfold, thats what you use if you are doing it wrong. Leave the little tricks and workarounds for those that only make parts that have to look good. If you actually have to produce the parts in a typical fabrication shop then use sheet metal and figure out how to make it work!!!!

Start with sheet metal from the beginning, leave a .1 degree gap and it will flatten.

[jefke1988]

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@Mario428 wrote:

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@jefke1988 wrote:

So you say it can Un-fold & Re-fold just fine?

I have no problem creating a flat-pattern of the part, just Unfolding & Refolding it.

I will give it a go anyways.

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No fold & unfold, thats what you use if you are doing it wrong. Leave the little tricks and workarounds for those that only make parts that have to look good. If you actually have to produce the parts in a typical fabrication shop then use sheet metal and figure out how to make it work!!!!

Start with sheet metal from the beginning, leave a .1 degree gap and it will flatten.

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I think you are not getting my point. We are making it work, but we want to make it work better. Standing still these days is the same as taking 10steps back. We try to tackle points that are time consuming.

(i can get a good flat pattern but i can only use it in 2D and not in 3D, and thats what i want)

Also fold & unfold is using sheet metal? It's not a trick or workaround.

For us it could be a way to nest plates on a unfolded cone, and see the nesting afterwards? Isn't that the whole point, that if you do something you get maximum result from it?

I want to nest my plates on the unfolded cone split them on the face and then refold them. So i can perfectly see where my weld seems are.

Then i need to rotate my roof that no nozzle connection are positioned on the weld seem.

Example:

There need to be 20 nozzle connections on this roof. Customers wants to change the position of a few connection? No problem we have markings of our weld seems and can instantly see if there is a problem.

(this example is a small roof with only 3 weld seems. In large case roofs are +40 meters in diameter and there are loads of welds.)

So i wonder why you call this a "trick/workaround" in my experience this is a usefully asset to a design process?

Further i tried the lofting technique and the result is not quite what i hoped for. We make our roofs without "bending" it and it gives a lesser result then my way of drawing for our use.

[Mario428]

Unfortunately we use different versions of IV or I could possibly show you how I would do something like your cone such that they were "smart" parts as I call them.  EG do the model and everything is right with the world and the flat patterns are correct without a bunch of effort.

How your shop forms the cone makes a difference is how the loft is done, can be faceted or smooth. Smooth if slip rolled to shape or faceted if bump bent in a press brake, Inventor will do both.

I have used Fold/Unfold before but only if there is a usable plane on the part, not an edge.

It is a last resort type feature for me because the results suck

If you sent a rough idea of what you are doing I could send you back stp files of what I come up with

[brendan.henderson]

Here is a link to my recent blog entry on this problem. Regardless of the method used to create the part it will fail, except for 1. Revolve surface and thicken works but only if the revolve is less than full (try 359.9 degrees).

I raised a support case on it. The bug seems to have been there since 2009!

[Mario428]

Interestingly I did it in 2014 sheet metal quite easily and it works quite well.

Yes there is a .1 deg gap, at a 60 inch diameter the gap is less than a 1/16, meaningless in the real world

[brendan.henderson]

Your part is not quite right as there is a flat section in Sketch8 & Sketch9. This changes the part setup when the Unfold/Refold is performed which allows it to unfold & refold correctly.

If you follow the steps shown in the blog the refold will fail repeatedly. It;s a bug acknowledged by Autodesk.

I have an Incident ID and have tried to update the content as I believe it's misleading but I can't (it has nothing to do with a cut and mitre). It's a bug in the refold when the swept angle is greater than 180 degrees (which means any cone with an included angle of more than 60 degrees).

[Mario428]

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@brendan.henderson wrote:

Your part is not quite right as there is a flat section in Sketch8 & Sketch9. This changes the part setup when the Unfold/Refold is performed which allows it to unfold & refold correctly.

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For a part to unfold and fold there has to be a flat to use for a reference, this is the biggest issue with the cone you all are playing with.

Quite simply you all do a really bad job of modeling a part and then squeal like little children when the software cannot do what you want it to do. I can only shake my head.

The cone I drew has a 1 deg wide flat that disappears when the part is actually made in the shop, as I stated the gap at the 60 inch diameter is 1/16 of an inch wide, meaningless in real life.

As always CAD discussion forums are divided between the people who model parts that can be made on the shop floor they work with and those who model "pretty" parts that no one can make but they are absolutely correct to the last detail. The fact those petty details cannot be translated to the real world is meaningless.

Rant mode off  LOL

[brendan.henderson]

The workflows discussed are just as valid as yours except that I don't need to employ what I consider is a a workaround (the small flat) to get it to work.

The reference flat you refer to can be the ends of the part representing the part thickness. Using this technique shows the flaw in the Refold in that it cuts off a section of the refolded part if a certain Unfold circumstance occurs. A bug has been found and documented.

A valid alternative has also been found to get past this problem.

Your assertion that "you all do a really bad job of modeling a part" is simply wrong. We are asking the software to do exactly what it was designed to do. Looking at your first supplied 1/3 cone I see that you have made extrusions in the Flat Pattern which don't occur in the Folded Part. Not acceptable for me.

Speaking for myself, you know nothing about me or my work or my manufacturing methods. The workflows used are all correct. If I use your part and put it's flat pattern on an drawing and turn the Bend Extents on then I see the 3 lines representing each of the bend positions. I would not put this out on the floor for manufacture. It is simply below my quality standards.

Take a chill pill Mario. No one is squealing.