Inventor: Trouble Fully Constraining a 3D Sketch

[andrewdroth]

I have a new co-worker who has been a Solidworks guy up until this point.

He was asking me how to fully define this 3D sketch, and I have no idea.

I searched the forum and found a lot of similar threads. Most of the time the solutions are to start with 2D sketches, or dimension to the origin planes. Surely there must be a way to use 3D sketches without doing that.

My co-worker tells me making 3D sketches is very easy in Solidworks.

I rarely start with 3D sketches, but now that I think about it, there shouldn't be any reason why it's so difficult to make them do what you want.

Does anyone have 3D sketching pointers? How would you constrain this 3D sketch?

[SBix26]

I'd say that your sketch is fully constrained, the colors notwithstanding.

I'm mystified by your use of Fix constraints, though-- wouldn't you want to constrain this to the origin planes?

In any case, if this is a skeleton for Frame Generator, why bother with a 3D sketch?  I would use a combination of surfaces and 2D sketches, which are much easier to construct and control:

Even though there are six sketches and a workplane involved, it is quick to construct and rock solid.  Yes, I agree the 3D sketch should show as fully constrained.  But this is so much easier!  This file is attached below (2019 format).

---

Sam B
Inventor Pro 2019.2 | Windows 7 SP1
LinkedIn

[marius.gildehaus]

Hello @andrewdroth!

You could also do it with a solid, in attach is my attempt on that

[andrewdroth]

---

@SBix26 wrote:

I'd say that your sketch is fully constrained, the colors notwithstanding.

It's not because as you can see in the screencast the bracing can flip.

---

@SBix26 wrote:

I'm mystified by your use of Fix constraints, though-- wouldn't you want to constrain this to the origin planes?

Like I said this is a new co-workers part. I just deleted the sketch on the origin and grounded the lines at the base to simplify the part and make it easier to identify the issue. Those grounded constraint's are not affecting anything.

---

@SBix26 wrote:

In any case, if this is a skeleton for Frame Generator, why bother with a 3D sketch?  I would use a combination of surfaces and 2D sketches, which are much easier to construct and control:

---

---

This is not for Frame Generator, it's for Autodesk Simulation mechanical and it's the only linetype that it will import form an ipt.

---

@SBix26 wrote:

Even though there are six sketches and a workplane involved, it is quick to construct and rock solid.  Yes, I agree the 3D sketch should show as fully constrained.  But this is so much easier!  This file is attached below (2019 format).

---

This is how I would typically model it, and then'Include' those lines in a 3D sketch. But my co-worker is right, you shouldn't need to do that in order to get a functioning 3D sketch. It's extra steps.

Thanks for looking though!

[JDMather]

There is no real difference between 3D sketching in Inventor and SolidWorks.

I recommend that your coworker continues to practice and carefully observe the behavior while sketching, and just like in SolidWorks - right click to find “hidden” functionality for power users.

If all else fails, Attach *.sldprt file here and I will create video demonstrating effective techniques.

[andrewdroth]

 Hey JD,

I'm being told that the the type of dimension I create in the 2D sketch in the screencast below is possible in SW. Can you confirm that?

As a side note, why doesn't the long line in the 3D sketch turn to a fully constrained color once the dimension is placed. And how am I able to swap the color of the rectangle by stretching nodes?

[JDMather]

I am going to be out of my office without access to CAD machine till Wed of next week.

If someone does not reply sooner - bump this back to the top to remind me that it is still open issue.

[andrewdroth]

Sounds good. Thanks!

[andrewdroth]

Hey JD,

Do you think you could look into Solidwork's ability to dimension this 3D sketch?

[johnsonshiue]

Hi Andrew,

Many thanks for sharing the case here! This is a bug I would say. I just edit the 3D Sketch and drag a line. Then all of a sudden the lines are all colored as fully constrained. It should not be like this. It should be shown as fully-constrained to begin with.

I will work with the project team to understand the behavior better.

Thanks again!

[andrewdroth]

Thanks Johnson!

[kelly.young]

Hello @andrewdroth I usually use Work Planes to constrain for definition instead of the lines themselves where I want my 3D Sketch to go. I found this way makes sure that the connections are where I want them and they do not flip as the offset values are positive or negative from the Origin Planes.

 Notice no dimensions on the lines, see if the attached part helps!

Please select the Accept Solution button if a post solves your issue or answers your question.

[ben.conway8USAC]

It is not constrained because there are two (or more) solutions to the set of dimensions in the sketch. In inventor line dimensions are lengths not vectors so there is no direction information. The 3D sketch below shows two such solutions. The two driven dimensions are dimensions from the plane (which do include direction and sign). all the other dimensions are line lengths. As far as I can tell there is no way in an inventor 3D sketch to force one solution over another. Add to this that Inventor is likely recalculating the solution from where the lines are dragged to not from the last good solution and things can flip if dragged closer to a different solution. A similar thing happens in 2D sketches if you change a dimension to 0 and then back to the original value. It seems to me to be fundamental to the mathematics that Inventor uses.

[Frederick_Law]

Do not use 3D unless you don't have a choice, like helix and coil.

3D sketch is as unstable in SW as in IV.

Frame member will rotate on the sketch randomly in SW.

Use 2D sketches and you'll have way less problem down the road.

And tell the new-b, stop thinking like SolidDoesn'tWork.

Start thinking like a Inventor.

Tell new-b there is one thing Solidworks is better and faster then IV.

It's crashing.