Revolve in assembly

[Cad4fish]

I will start by admitting I have not gone through all the Inventor tutorials.  I've just jumped in and been able to create several parts and assemblies.  Now I am stuck.  I want to visualize how a turned bottle stopper will look if the blank is made up of a stack of wood with alternating colors of wood and then turned to roughly an egg shape.  I may be at a dead end because from what I can tell the join/cut/intersect options for revolve are not available in an assembly.  I am attaching what I have so far and would like to know if there is another way to accomplish this.  With a derived part the stack of blocks becomes one part so I can't see what the colors will look like.

[admaiora]

I see a lots of thing that they would suggest you to pass before through the tutorials

For example in the assembly, just ground least a component, you can't assemble with a not stable and moving group of parts.

For your egg cut..you want to cut all that parts, so the sketch has to be created at the assembly level and not in the part 3.

So, at assembly level > 3D Model Tab > 2d Sketch > revolve etc etc

[WHolzwarth]

And you can do that with much less work. See file (2015)

[wimann · Accepted solution]

I've mentioned this before in some of my other posts, but while I can't open your assembly since it's in 2015 and address it directly, one thing I would suggest is a multi-body part. Granted that in your case, it is somewhat beneficial to be able to reuse two part files and constrain them over and over to get your stack of word instead of having to create multiple solid bodies, solid bodies offer the flexibility of easily applying the change your intending to apply as well as the ability to make a detail sheet of the individual cut parts.

I'll attach a part file and try to give some instruction on how it is done.

I'm just going to touch on two of the key points:

1. When extruding, you have the option to Combine, Cut, Intersect, or New Solid. You're probably quite familiar with the the first 3 but the last one is used less often. It creates a separate entity in the same part file that can be used in many different ways. In this case, I want to make each block of wood seperate so that they can be exported out into any assembly then perhaps detailed on a drawing. In my first image, I've highlighted where this button is. Part of my process is first creating each individual block. Time consuming? A little. But this process makes up time on the back end.

2. My revolve cut that creates the egg shape is set to include all solid bodies by first setting the revolve to cut then ensuring that all solid bodies are selected (in that order). You'll notice in my second image that I highlighted where you selected the solid bodies to be included in the feature. This button only appears in the feature dialog when multiple solid bodies are present in the part, otherwise you my have never seen it before.

Other than that, snoop around. I used a few equations and driven dimensions to help hold everything together and to also make it all relate to one another. If you want to make parts out of the solid bodies you can go under your manage tab and select either "Make Components" or "Make Part". Make Components will generate parts out of all the solid bodies you select as well as an assembly where all your parts will be pre-placed and grounded based on their location in the original part file. Make Part will allow you to export a few solid bodies at a time and make part(s) out of them individually but won't place them in an assembly for you.

Hope this helps.

[JDMather]

Will, that looks like too much work to me?

[wimann]

JD,

I agree that it's more work up front but, unless I'm mistaken, if he does the revolution in the assembly, doesn't it not effect the individual .ipt's (opened and used outside of the assembly) and if that is so, he wouldn't be able to make the individual details on a drawing. That's the advantage I'd be looking for. Other than that, the multi-body part way offers the same flexibility as the assembly with the help of the equations used in it aside from when you add more wood blocks.

It may just be what I've adopted from my own work experience, but I tend to stay away from assembly features where I can. They can save time on the front end but when I've got to detail something out, unless there's something I'm missing, I end up having to go back and apply the features at the part level anyway.

If there is something I'm missing, feel free to let me in. I'd love to know.

Thanks,

[JDMather · Accepted solution]

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@wimann wrote:

JD,

I agree that it's more work up front but, ...

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I was only referring to how you created the Multi-body and how I created the Multi-body, not referencing assembly operations.

Check the construction of the file I attached above.  All controlled by 1 Parameter (Block_Size).

[wimann]

Aha! That's what I was missing. See, I was under the impression that when you selected to create a new solid in rectangular pattern that all the occurances were grouped into one new solid. In other words, I would have thought that the outcome of your pattern would have been two solid bodies. But with that misunderstanding ironed out, the rectangular pattern is definitely the way to go.

In fact, that's the only reason I did the pattern in the sketch. Otherwise I stray from sketch patterns as well.

Thank you for that. Actually makes my day a bit better knowing that the way you've done it works. Now I can apply it elsewhere.

[Cad4fish]

In my very first attemp I did a pattern of the first part but was not able to change the color of the parts individually.  I am attaching two images to show what I got when following wimann's instruction with a smaller group of parts and a simple half-circle.  The pattern was on the sides, but the curved section was all one color.  When I tried "Make Components", I was back to the same problem of only being able to cut with the revolution and just had a void in the center of the array of parts.

[JDMather]

So where do you want to do the cut?

Are you OK with doing at part level with multi-body solid

or

do you want to do it at the assembly level?

[wimann]

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@Cad4fish wrote:

In my very first attemp I did a pattern of the first part but was not able to change the color of the parts individually.  I am attaching two images to show what I got when following wimann's instruction with a smaller group of parts and a simple half-circle.  The pattern was on the sides, but the curved section was all one color.  When I tried "Make Components", I was back to the same problem of only being able to cut with the revolution and just had a void in the center of the array of parts.

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Are you certain you made the parts individual solids? The different colors are set by expanding the "Solid Bodies" folder in the browser (only present when multiple bodies are present) and selecting the bodies individually to change color. In my example, I set the part color to white and then selected every other solid body and made them some... wood color (I don't remember). I'm a little confused by what's going on with your half circle. If you've done a revolve cut and cut away all excess material on all solid bodies, I can't imagine why this wouldn't work. And once you use Make Components, your parts will already be cut because of the revolve cut in the initial part file. I'll attach a zip re-using my part file which, in case it's overlooked by anyone, can be done more efficiently (see JD's post).

[dan_inv09]

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@Cad4fish wrote:

... just had a void ...

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When I read that, and looking at stopper test 2.jpg, I start to think the problem is only that we're trying to cut away what is outside the profile. (I wish I could look at the files; we will upgrade from 2014 as soon as they sort out the server - last time that was the case we jumped two or three releases.)

If that's the case you just need to make an "outside" to your sketch (don't forget to make it bigger than the corners).

It would be nice if we could cut everything outside of the profile, but for now you can only cut what is inside of something on your sketch.

[JDMather]

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It would be nice if we could cut everything outside of the profile, but for now you can only cut what is inside of something on your sketch.

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Wouldn't that be the same as Intersection with the inside?

There are only two simple sketches in the example I attached - cut away all outside of Sketch2.

[wimann]

If only we could use that with multiple solid bodies.

[JDMather]

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@wimann wrote:

If only we could use that with multiple solid bodies.

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I think you will need to qualify that further - there are multiple solid bodies in the file I attached.

[wimann]

So I learned two things today. 🙂

[dan_inv09]

That's not an assembly, is it?

[JDMather]

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@dan_inv09 wrote:

That's not an assembly, is it?

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No, only Cut is available in assembly, not intersection.

Looks like there was some confusion about what environments we are in.

[dan_inv09]

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@Cad4fish wrote:

... When I tried "Make Components", I was back to the same problem of only being able to cut with the revolution and just had a void in the center of the array of parts.

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That's an assembly - and "only being able to cut with the revolution" kind of spells out that you can't use intersection.

(I never use intersection, it just takes three little lines with dimensions - but I'm not going to lie to you, if you had asked me what that button did 10 minutes ago I wouldn't have been able to tell you.)

[Cad4fish]

I was able to create the pattern and revolve/intersect and get a ball made up of the individual occurances of the feature.  What I still cannot do is change the color of the individual occurances.  I will attach an image of my model tree.  It is different than yours. (I am using v2015.)  Does anything here indicate where my problem lies?  As for do I prefer to do this in a part or an assembly, I don't have a preference.  It seems from all the posts that I should be working in a part and that is fine for me.