revolve nonsense - autodesk saying "As designed"

[kmeldfreyssinet]

Hi all,

I decided to bring this to forum because from subscription help I am getting answer I can not accept.

The thing is I want to create simple con surface using revolve command. Only I need to create it in not very usual situation.

I enclose ipt file with geometry set up.  In this file situation is as follows:

1) sketh 1 is defined in XY origin plane and it contains two ortogonal lines. one line starts in the middle of secound one. This two lines represent directions of "slope line" and "level line" of some plane. Originally this plane is defined by other geometry but for purpose of this exumple I define it. In real situation this plane is given.

There alse is a point defined that dose not beling to any of this straight lines.

2) 3D sketh 1 defines a point directly over the end of "slope line" defined in sketch 1. this point is 100 above XY plane

3) work plane 1 is defined using "level line" (the one in the middle of witch starts the other one) and a point defined in 3D sketh 1. In real situation I start my task from here, this plane is given.

4) Work axis 1 is normal to work plane 1 and go threw point in the middle of "level line" of workplane 1. So this point belongs to this work axis, and therfore it croses "level line". In consequence this two lines lie in some plane (ar coplanar)

5) 3D sketh 2 defines a point 200 over XY origin plane directlly over point defined in sketch one. This point is not in work plane 1

6) Work plane 6 is paralel to XY origin plane and goes threw point defined in 3D sketch 2

7) Work point 1 is defined in place that Work axis 1 meets work plane 6. So this point belongs to work axis 1.

😎 on Work plane 6 sketch2 is defined. Work point 1 is projected on the sketh, but since Work point1 lies in sketch plane it's projection in precisly in the same place in space as point itself.

Also point defined in 3D sketh2 is projected to thisketh2, but since this point also lies on work plane 6 which is plane of sketh2, projection of this point and point it self are precisly in the same place in space.

Than there is a line starting in point being projection of point defined in 3D sketh2 and doing in the direction of projection of work point 1 (which also lies on work axis 1).

In consequence line defined in skketh2 crosses work axis 1 in work point 1. Therfore this two lines are coplanar but not propendicular.

What I want is to create conical surface by revolving line from sketch2 around work axis 1.

Pleas try to do so. You will be suprised.

If you had tried you see that revolve was not done around work axis 1, althought you was able to select it as revolve axis.

Also this operation is perfetly ok in terms of theory because this two straight lines are coplanar. They are because they are defined in such a way.

I had send this, as a bug to subscription help and after some struggle I got a answer that this works as designed.

In my opinion it dose not at all.

Could you join me and also send this to Autodesk.

Regards,

Cris

[-niels-]

I was somewhat surprised, but i can understand it being "as designed".
It seems the direction of the workplane's axis goes before the the direction of the revolve function.

Your part already had the required steps to get the result you want, so am i right to assume this is more of a plea for autodesk to change this behavior?

If so, i think your best option is to put it on the ideastation and describe the problem and how you'd like to see it changed.
Add pictures and such to make it a compelling idea for other users to cast a vote on.

If you do, add a link to it in this topic if you like.
You'd get my vote, because "as designed" isn't always what you'd expect to happen. 😉

[wilkhui]

Hi Cris,

I'm looking into this and will get back to you shortly.

Thanks,

Indy

[Daniel248]

...

"What I want is to create conical surface by revolving line from sketch2 around work axis 1."

...

Hi Cris,

Not sure it helps with the behaviour of revolve command, but, by creating a new plane defined by the two elements (line from sketch2 and work axis 1) and creating a new sketch on this plane by projecting these two elements, one can revolve the line around the axis using this new sketch. Modified part attached.

Regards,

Danny

[johnsonshiue]

Hi! This is an internally imposed restriction, not a technical limitation. Inventor's assumption is that Revolve command only works for 2D Sketch profile and co-planar axis. However, mathematically as along as there is a profile, any axis in the space should help define revolved geometry.

Revolve is a special kind of Sweep. Actually, you can create the desirable geometry by creating a circular path on a plane normal to the intended revolve axis.

Thanks!

[kmeldfreyssinet]

Hi,

replay to johnsonshiue

When I went to help to see if there are any restriction to revolve operation listed, I found there are non such that should make revolve in my case to be impossible. It is clearly stated:

          "Selects the axis of revolution. The axis can be a work axis, a construction line, or a normal line."

So it is not said that it has to be coplanar with selected profile (I remind that in my case this two lines are coplanar). I understand coplanar as strictly coplanar that "lay in the same plane" and not nacasarly plane of sketh line is createn on.

It is also explicitly said that it can be "work axis" what is the case in my example.

So in terms of limitations you mention they are not listed anywhere where could be found by the user. Also they are not obayed by the program because I was allowed to select this axis. In consequence I got result, which is created surface, that is not correct. Case that I had define has one and only one correct solution, and it is not the one program produces. There also is another thing. If you get surface that Inventor produces in this example actual axis of this surface is nowhere near work axis 1 which was selected as revolution axis. In any case they should be the same. If they are not it should be found and I would expect en error message. If program produces something against accepted input I consider this a bug. I could compare it to a situation in which I would order calculator to do following equation 2+2*3 and got result of  because it has certain limitations that would be"you can use multiplication operator and others but no matter what you do all operators will be treated as addition. Would you like to use such a program?

I wander what if I had situation in which difference between my worklane 1 and XY origin plane was so small that I was not able to catch difference between what program did create and what program should had create. Currently I am not confident at all about results gained from Inventor. If it has such a bug it as well can have others in different places. like for example on I found some time ago in sterss simulation.

http://forums.autodesk.com/t5/Inventor-General/stress-analisis-worning/m-p/3054546#M404691

replay to general:

Daniel248 thanks for suggestion. I did this because I needed to construct this con. I am doing well enough in geometry to finally get what I want.

What I am trying to point is that if I pay a lot of money for the program I expect this program to help me and not to force me to do extra tasks, for example to define two extra work planes and extra sketch to perform simple geometrical operation (old autocad could do that in 3D).

Revolve in one of most simple and basic operations you can imagine in 3D. Therefore I expect this to work properly, and I discover something opposite.

Regards,

Cris

[glenn-chun]

Hi Cris,

As a former ASM developer, I would like to show you what axis Inventor passes in to ASM (geometric modeling kernel).

In your rev nonsense.ipt, Inventor passes in the red axis to ASM:

 

The profile plane for Sketch2 does NOT contain the user-selected axis.  I'm not sure if the Inventor's behavior of creating the red axis is as designed or an undesirable byproduct due to the precondition that is not met.  Maybe some Inventor developer could chime in with a comment.

As for Danny's rev nonsense (1).ipt, Inventor correctly passes in the user-selected axis to ASM.  Note that the profile plane for Sketch4 DOES contain the user-selected axis.

Solution 1 (using Revolve): Make sure the sketch plane for the linear profile contains the axis of revolution.

Solution 2 (using Sweep): Create a circular path on a Work Plane normal to the axis.  Make sure the path intersects the linear profile.  Sweep the linear profile along the circular path.

Glenn

[kmeldfreyssinet]

Hi,

thanks for additional information. This may show actual problem I am after and Autodesk seems not o see.

I know that my sketch plane dose not contain work axis 1, but in the same time line I want to revolve is strictly coplanar with work axis 1 (in space).

I am not export in programing but just a user of this software. I therefore should not be expected to get in to how software gathers and passes data to kernel. I could be expected to do so in case of opensorce software with no, or limited documentation.

The thing I am fighting is that software costing a lot + subscription cost dose something like I showed and no one seems to feel responsible nor is willing to do anything except living my with "as designed" statement.

I would except situation in which AI would say "not able to revolve" or " self intersecting ...." or "inconsistent data" even. Than I would say "you should add this functionality because your competitors haw it". But now program is doing something that it should not do in any case, that is using data not consistent with user input. Which, for me, is obvious bug.

Regards,

Cris

[glenn-chun]

Hi Cris,

I logged a defect against this issue:

DID 1517846: A wrong surface is created when a linear profile is revolved, depending on the sketch plane.

Hopefully, Inventor team can confirm and fix this defect in the near future.

In your rev nonsense.ipt, Inventor internally uses a *projection* of the original axis onto the *sketch plane* that the linear profile is created on.  I don't think that's a right behavior.

In my opinion, the right behavior should be the following: If there exists a plane that contains both linear profile and the axis of revolution (Let's call this PlaneX), then Inventor should use the original axis, regardless of whether the sketch plane of the linear profile matches to PlaneX or not.

Currently, Inventor creates the correct revolution surface only for the case of Sketch Plane A, which is the same as PlaneX.  After the defect is fixed, all cases (A through F on the figure above) should create the same revolution surface shown below:

Glenn

[kmeldfreyssinet]

Hi,

I also reportet this and my case number is CaseNo:09602684

Cris

[ravikmb5]

some how i was able to Revolve sketch2 line around workAxis1

Attached

is inventor 2015 ipt File

[kmeldfreyssinet]

Sorry but you was not.

In your solution Revolve is done around projection of work axis1 to skethch2.

If you examine file you attached you will find the difference between work axis1 and line projected to sketch 2. (Although you probably did not project it intentionally, Inventor "did it for you", although you really did not want it to do that).

I attache part in witch I have created proper revolve surface.

So this bug is still a bug.

Cris.

[Echoo]

I am agree with you , this is big bug 
another software has mpre great geometri solution 

[TheCADWhisperer]

---

@Echoo wrote:

I am agree with you , this is big bug 
another software has mpre great geometri solution 

---

You did not attach file from "other software" to illustrate your statement.

[Cris-Ideas]

---

@Echoo wrote:

I am agree with you , this is big bug 
another software has mpre great geometri solution 

---

I would be very interested too to know what software you have in mind.

Cris.

ps. this is my old thread started from previous account.