Can't I constrain a part to an assembly sketch?

[Anonymous]

I have a fresh new assembly with a sketch as a feature in it.  I then assemble some parts into the assembly.  I cannot seem to select any of the geometry in the assembly sketch to constrain any parts. Is that how it is supposed to work?  I cannot even create work features using the sketch.

[JDMather · Accepted solution]

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@Anonymous wrote:

... I cannot seem to select any of the geometry in the assembly sketch to constrain any parts.

 I cannot even create work features using the sketch.

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Create a dummy part (typically named Skeleton or Master) with part level sketch.

Assembly level features are subtractive (Cut) only - same as in real world.

Perhaps what you really want to do is Edit your part in the context of the assembly?

[Anonymous]

Thanks @JDMather for responding.

I was hoping to avoid another file associated the assembly created by using a skeleton part.  I could make another part with the sketch in it - but I do not need to for this assembly.  I want to use the sketch created in the assembly as the skeleton.

My question started out because I want to align multiple parts to a sketch I created in the assembly.  Nothing to do with editing parts at this point - but hey, now that you mention it, I want to do that too!

[johnsonshiue · Accepted solution]

Hi Ronald,

The ability to constrain to assembly sketch geometry is not available yet. Assembly work geometry cannot be created on assembly sketch geometry for the same reason, because assembly work geometry is constrained to the geometry it is associated to.

Assembly sketch is mainly built for creating assembly features. Could you tell me why you have to use assembly sketch to constrain to something?

Many thanks!

[Anonymous]

@johnsonshiue when you say "YET", does that mean it is going to be available?

I want to use an assembly sketch as my skeleton instead of another part.  One less file to manage.

Thanks.

[johnsonshiue]

Hi Ronald,

I knew people would interpret "yet" extensively. It is indeed not available yet. But, I cannot comment on when it will be. Never say never. Let me work with the project team and see what we can do about it.

Many thanks!

[Anonymous]

Sounds good, thank you!

[Anonymous]

One very good reason is to be able to constrain prototype tooling parts to a chain or cam track that is defined by a sketch profile only, rather than having to make dummy parts with the features and using tangent constraints.

You can do this in Solid Works.

[johnsonshiue]

 Hi Nathan,

Great point! I was not aware that our competitor had the ability. Regardless, it is true that it is still not yet available in Inventor as of 2019. Let me work with the project team to understand the request better.

Many thanks!

[Anonymous]

I used Inventor for 8 years then Solidworks for a year and now back to Inventor. In Solidworks I learned to make sketch driven assemblies. I can build new parts and constrain existing parts to the assembly sketch. Not only was this top-down approach more intuitive, but sketch driven assemblies are very easy to manipulate after they are built. I've tried to make some sketch driven assemblies last couple weeks using Inventor and it has not worked out, that is why I'm reading this forum (mainly because I realized the part is not constraining to my sketch).

Another feature that I miss greatly (Solidworks had this feature by default): being able to select a plane on part A and plane on part B, then constrain menu automatically pops up and usually has the correct constrain chosen with the distance parameter ready to be typed in (I don't have to choose the constrain menu nor do I have to click on distance - I just start typing distance). Solidworks is setup like this by default - doing a 100+ constraints a day, less clicking saved me a great deal of time. What is important, it is by default, no setup needed.

Another feature I miss which is sooo simple and a default in Solidworks that I took for granted, any line I click on a part (regardless assembly or part file), in the bottom of the program window frame, it shows the distance. I don't have to do extra clicks for measure tool (nor do I need another menu taking up space). If I needed more data, then I would click measure tool. If I remember correctly, if I click two surfaces, it would also show the angle.

Inventor has lots of potential - but I wish it moved away from hot keys/menu clicking and more towards anticipating what the user is trying to do and filling in the gaps automatically. This can be realistically done with common tasks like constraints.

[johnsonshiue]

Hi! I appreciate your feedback and your comments on our competitor. It is very helpful. This particular thread is about selecting assembly sketch on creating an assembly constraint. The ability is not yet available. There is room for improvement in every corner of Inventor. So are our competitors. If you have other comments, you may want to start a new thread.

Thanks again!

[Anonymous]

you used to be able to constrain parts to sketch geometry within other parts. was doing all the time prior to 2019.

[JDMather]

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@Anonymous wrote:

you used to be able to constrain parts to sketch geometry within other parts. was doing all the time prior to 2019.

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Attach your assembly here.

[johnsonshiue]

Hi Robert,

Yes, users are allowed to constrain a piece of geometry (body or skech) within a part to another piece of geometry within another part. But, you cannot constrain a part to an assembly sketch. Or, you cannot create an assembly level work feature based on an assembly sketch.

If above statement is not true, please share an example and I need to understand the behavior better.

Many thanks!

[Anonymous]

I have parts constrained to sketch geometry within 10209-MASTER SKETCH.ipt

However the ability to do this stops working after a few parts have been added.

Restarting Inventor fixes this temporarily 

[johnsonshiue]

Hi Robert,

Do you mind showing me how to see the failure?

Many thanks!

[Brandon_Mooney]

I know this is an old thread, but for those of you like me who need to use alternate constraints that are related to a customer requirement via a sketch in the assembly, you can get around this by referencing a sketch dimension in your constraint.

Example:

1. Make your .iam

2. Create a sketch in the .iam

3. Create a point in the sketch where you wish your part to be constrained to, and dimension it from a projected line that you know will be constant to how you wish to constrain your part.

4. Take note of the dimension's label (ex. "d142")

5. Make a constraint from the project plane or axis (the projected line in the sketch) that uses the same dimension ("d142")

It's roundabout, but lets you constrain parts with sketches while that functionality isn't yet implemented.

[Anonymous]

@Brandon_Mooneythanks for the tip.  I just searched this issue yesterday and found my old thread.  I wish I had some sort of idea what Autodesk was working on.

Thanks

[saurabh.lahamate]

I want to create Animation Timeline for an assembly. Creating a redundant part(s) creates a lot of complications as some parts in the assembly are adaptive and some virtual. Is an option available now, in Inventor 2020, to constraint parts to a skeleton in an assembly sketch. This will aid by treating parts of those sketches as parameters to create a smooth timeline. If no, what is the next best option to do so.

[johnsonshiue]

Hi! The short answer is no. Assembly constraint does not support assembly sketch. It has to be part sketch.

Many thanks!