Unable to Revolve/Sweep a Solid in Inventor 2016

[saru_ks]

Hello Friends,

I am a Newbie to Autodesk Inventor and just about a month in the learning curve. This is my first project on Inventor for submitting to college. Its a simple assembly as shown in the attached pic. It has two platters at 60 degree angle to each other with 6 rollers supporting it on the outside edge.

My issue is I am having difficulties cutting dimensionally accurate grooves in the rollers. I tried revolving a sketch with calculated values but inventor reports interference when I run a interference check. I also tried projecting cut edge to the sketch which gave slightly less interference. So currently I am trying to revolve a Solid around the edge where the roller needs to be grooved. However I am unable to use the Revolve or Sweep tool to do it. I have attached the part file. The Solid which is used to cut the groove seems to be attached to the roller. It might be due to "New solid" option selected during extrusion of part of the platter to be used as the cuttting tool. Please help me to understand what I am doing wrong. Please tell me the right way to revolve that solid to cut the groove in the roller.

I have attached the part I am working on and which would be at 4oClock position in the assembly.

Please excuse me if I have not used the proper technical terms. 

Thank you in advance.

[Xun.Zhang]

Hello @saru_ks,

Because you are working on a multi-solid part, you have to pick up a solid to merge with.

Try to pick a solid before revolve, please check out the enclosed file for reference.

Or you can simply create new solid by check the New operation, hope it helps!

[saru_ks]

Thank you Xun Zhang.

Wow!! That was a Fast response!! Thank you so much!!!

In the solution you provided, you have revolved the sketch left over from an earlier projected sketch. I am interested in knowing how I can revolve the solid (attached to the roller on the other side).

For you to understand the design intent I will attach the assembly file below. In the assembly you can see one of the roller grooved. I am trying to groove the other 5 rollers similarly but running into interference issues.

[Xun.Zhang]

Hello @saru_ks,

Re-attached, please check it out.

Hope it helps!

[saru_ks]

Thank you again for the fast response.

The solution which you have suggested in the assembly you sent is not what I need. Maybe I was not clear what I am trying to do. Please see the attached pic.

In simple terms, I am trying to rotate the solid(as positioned) around the axis of the roller and remove material so that a groove is created similar to the one shown in the pic below.

Is it possible in Autodesk Inventor????

[TheCADWhisperer]

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@saru_ks wrote:

...This is my first project on Inventor for submitting to college. ....

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When I examine your Sketch1 in the part - it does not appear to me that you are recieving proper instruction in how to use Inventor. Can you ask your instructor to join this discussion?

[WHolzwarth · Accepted solution]

I didn't look at your way of modeling, but attached is an approximate shape of the groove (2016 IPT).

Shape is getting better with increased number of pattern members. (IPT: 60, Screenshot: 360)

[saru_ks]

Thank you Walter!! Thats exactly what I am trying to achieve!!!!

I had a look at your attached part file. You have used the circular pattern tool. My knowledge of the circular pattern tool is very basic. I will try to duplicate your approach and let you know my results at the earliest. 

Thank you so much for pointing me in the right direction!!

PS: Pardon my NOOB question, but is it not possible to revolve a solid part using the revolve command??? Or is revolve limited to Sketches??

[saru_ks]

Thank you CADWhisperer. I agree with you that I probably need to grab a few basic concepts. I am at the very beginning of the learning curve. I could ask my instructor to join this discussion, but as of now I would rather learn from other resources like this forum. Maybe it would give me an opportunity to understand how an Experienced Engineer like yourself would approach this issue. Walter has sent me a part file which is close to what I am trying to achieve. I will use his approach and let you know how it turns up.

Thank you again for your time!

[TheCADWhisperer]

I notices a large number of 90° dimensions in your Sketch1. 

You should never ever have a 90° dimension unless the Design Intent might call for the angle to be changed.

Inventor should have added Horizontal or Vertical or Perpendicular constraints to the lines for you.

Sometimes you need to manually add these constraints (rather than dimension angle of 90°).

You have extra work planes and sketch geometry.

I suspect there is a far easier, more robust solution than Circular Pattern to achieve your Design Intent.

Also, your school (and you) can get the latest version of Inventor for FREE from http://www.autodesk.com/edcommunity

[saru_ks]

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@TheCADWhisperer wrote:

..... I suspect there is a far easier, more robust solution than Circular Pattern to achieve your Design Intent.

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You are right. Walters approach does show one way to approach this design and gives me few inputs to get some measurements to try and modify the base sketch. However as you said there must be another solution. That is what I am also trying to find out. Do you know of a better approach??

The 90 degree angles, missing constraints and manual dimensioning are Newbie mistakes or lack of experience. My plan was to complete the design and ask my instructor to correct the mistakes. However if you could point me to additional resources to hone my Inventor skills, I would appreciate that.

Thank you for letting me know about the free Autodesk Inventor download. Unfortunately the computers in my school are a little outdated. I am not sure if it would support the latest version of Autodesk Inventor, but I will ask my Instructor to check.

Thank you for your quick reply and your time.

[WHolzwarth]

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@saru_ks  schrieb:!!

PS: Pardon my NOOB question, but is it not possible to revolve a solid part using the revolve command??? Or is revolve limited to Sketches??

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Hi Saru, actually Inventor can only do Revolve with sketches around a rotation axis in the sketch plane.

I can think of enhancements:

a) Revolve of sketches around an axis in 3D space

b) Revolve of solids  around an axis in 3D space

Perhaps Autodesk has similar thoughts. Time will show.

Right now, the only workaround I know is circular patterning. Version a) could be thickening a boundary patch of the sketch to a thin solid and patterning this

[WHolzwarth]

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@TheCADWhisperer  schrieb:

I suspect there is a far easier, more robust solution than Circular Pattern to achieve your Design Intent.

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Hmm, Jeffrey. Perhaps like that:

- Circular pattern only with 10 deg angle

- Loft or boundary patch along the outlines

- Sculpting these surfaces

- Pattern this with 36 members to 360 deg

Well, it's a thought. But I didn't try it.

[johnsonshiue]

Hi! Strictly speaking, Inventor 2019 and earlier is not capable to Revolve or Sweep a solid body along a given path. In some cases, you can emulate it by using a 2D profile but in many cases, this emulation does not generate the correct solution. We are aware of the deficiency and we are actively working on a solution. The particular case you mentioned is one of the cases that we are targeting to support. If you are interested, you can learn more at Inventor Beta site (sign up at https://bit.ly/InventorBeta).

Many thanks!

[saru_ks]

Hi Walter.

A quick update. I am using your approach to get the dimensions for the cut from the Patterned/Combined part  which you have sent. I am planning to use those dimensions to create a fresh sketch geometry and revolve it to derive a functional part. I got the dimensions for the straight edges. Having difficulty with the curved edge since its not a circular curve. My guess is its Parabolic curve. Since I am newbie and not too good in quadratic equations I would need some more time to figure it out. I will update you once I finish. Please bear with me.

Thank you for your time, patience and valuable inputs.

PS: I know that the curve need not be geometrically accurate to derive a functional part, but would still want to use a curve with a equation ("Equation Curve" in Inventor), so I get a deeper understanding of how the shape is derived.

[TheCADWhisperer]

What is the purpose for the cut?

Is this merely for clearance with another part when mechanism revolves?

What is the tolerance for your manufacturing process for all parts relative to this feature?

[saru_ks]

I was afraid you will ask me exactly these questions! 😉

Looking at the cut from a functional perspective, it does interact with the other part which it is driving. Practically speaking though, we can make it redundant (and use it "for clearance") so that a tighter tolerance is not required.  

I have never produced a part before. I am not sure of the tolerances to use. In layman language i would say that ideally this part should have "tight tolerance" at this cut and maybe "looser" tolerances as far as other dimensions are concerned. I was planning to consult my Instructor at a later stage. Should I work out the tolerances at the designing stage itself??

PS: I would be asking a professional CNC machining company to manufacture the part. Maybe I should check with them the tolerances their manufacturing process offers.

[TheCADWhisperer]

What is the purpose of this part?

What is the purpose of the assembly?

[saru_ks]

The purpose of this part (roller) and other 5 rollers in the  assembly is to hold the two platters in the assembly at exactly 60degree angle from each other in the horizontal plane.

The assembly is part of an experiment where light/laser would be refracted by optical components placed on the platter.

PS: The design is incomplete. We would be redesigning the 3mm sheet part which holds the bearing and rollers to accomodate a path for the light.

[TheCADWhisperer]

Ah, I didn't notice that you had attached the entire assembly earlier.

Now I have a better idea of your Design Intent.

I see a number of issues, but unfortunately because you are using a very old release of Inventor I am going to have to bow out of this discussion because you would not be able to open my later version files.

Keep in mind - out on the shop floor we cannot manufacture perfect parts, so include appropriate clearances right up front in the design considering the manufacturing and assembly tolerances.

Fully define each and every sketch (I also notice a lot of extraneous geometry creation).

Here is just one example (there are dozens if not hundreds of others in this assembly).

A 3mm plate will not fit into a 3mm slot, and in any case - we cannot make a 3mm plate or a 3mm slot (there will be manufacturing tolerances associated with each feature).

Not Possible