Distorted Element

[PrntMster]

Hello-

Could someone give me some guidance as to why the attached file displays the rectangular extrudes as it does? I.e., on my computer screen the extrudes appear mitered in depth. When the half cylinder is rotated to a level, side view, I do not notice the distortions. When I view it from a ve.yr slightly rotated plan view the extrusions appear to be present but also appear to take on irregular depths and are barely noticeable.

There appears to be some issue with the revolve. I created the larger initial half extrusion first, then added the holes and rectangular extrusions and at that point all features appeared correctly. At the point the revolve was added all other elements disappeared from the half cylinder (view wise.) The sketches along with the particular feature were still present in the model tree. After deleting the original sketches (holes & rectangles), then re-creating them after the revolve, they somewhat show up the rectangles appear distorted.

Any thoughts as to what I am doing wrong would be greatly appreciated.

[JDMather]

That is an interesting one.

Have you tried recreating totally from scratch?

Looks like simple geometry that should not cause this anomaly.

You might install SP1.1 and Update 2, but I don't think these have anything to to with the anomaly.

[PrntMster]

I have Mr. Mather. I have even tried different ways of creating the base object, i.e. extruding a full cylinder into a half, then adding features, extruding the half cylinder from a square block . . . .

It's weird in that the extrusions display perfectly it seems until the revolve is added.

I will try your suggestion of the servic packs and see if that may correct the problem.

Oh BTW, your work here on the web has been immensely helpful to me to be able to learn Inventor. Without it Inventor program would probably be useless to me. Thanks for your unselfish contributions and time that it has taken and does take to do what you do!

PrntMster

[JDMather]

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@PrntMster wrote:

I have Mr. Mather. I have even tried different ways of creating the base object, i.e. extruding a full cylinder into a half, then adding features, extruding the half cylinder from a square block . . . .

PrntMster

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So you are saying you started a new file and could reproduce this behavior from scratch?

I did not expect this to be a re-producable behavior.
I will have to give it a try myself and see if I can reproduce.

[PrntMster]

Yes sir - It has been reproduced in every new file while trying different methods of producing the base part (half cylinder.) As I said there seems to be some issue when the revolve feature is added that causes the problem.

I have just downloaded and installed SP 1.1 and the update. I will see what effect that may have on it.

Do you think the distortions would be reproduced in the actual part when the machine prints it out? If not I don't know that it is that big of an issue to me.

Thanks,

PM

[PrntMster]

Here is one that was built after installing SP 1.1 and update. Extrusions 2 & 3 were drawn before the revolve. They displayed perfectly. Added the revolve Extrusions 2 & 3 disappeared from the 3D view. Added extrusions 4 & 5 after the revolve, one seems to display Ok the other displays only half way.

[JDMather]

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@PrntMster wrote:

Do you think the distortions would be reproduced in the actual part when the machine prints it out? If not I don't know that it is that big of an issue to me.

PM

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I saved the part as *.stp and then opened it back up and the anomaly was not there.
I didn't try as *.stl

but I think this is just a graphics error in Inventor.  I don't think there is a problem with the geometry.

Because you mention printing I assume you will be saving as stl file.  You might save as STEP, import and save again as stl just to be sure.

[adsk_loren]

Hi,

The problem is caused by the extra lines near the arcs in the Revolve sketch. It looks like you started with a larger sketch profile and then changed the dimensions to make it smaller. You didn't clean up the geometry afterward, so there are some weird artifacts.

1) Change the .063 dimension across the arcs to .03. You'll see the straight line that connects the end points of the arcs.  It's hard to see at .063, but the arcs actually cross each other.

2) Zoom in on the "intersection" of the arc and the angled line. You'll see extra lines that form a V shape.

I found the problem when I deleted the flat face of the half round extrusion and tried to create a boundary patch. When I started selecting the edges, I couldn't select the second arc because its endpoint wasn't connected to the first arc. Once I knew where to look, it was easy to find the sketch problems.

Also, I didn't check the whole sketch. There might be other issues that aren't obvious at this scale.

[PrntMster]

You got it loren! I revised the fillet to a minimum .03 radius and whala - problem solved!

Now my question is why? Why doesn't the program prompt you to that theoretically it's not possible to place a .0313 radius on a .03 length line? Why does it manifest itself in the form of a distorted 3D image? Also, would you explain a little more about "cleaning up the geometry."

Thanks to y'all - loren & JDMather for your efforts in helping to solve this problem.

PM

[rhasell]

I am impressed.

I will remember this for future debugging of other users parts.

Only after going through the fix, did I notice the line in the fillet.

See attched files.
1 = OP part

2 = Loren fix.