Lock a Body in position?

[j9lemmon]

Is there a way to lock a Body in position? I sometimes get a message saying a Component has been moved, but I did not intentionally move it. I'm asked to continue or Capture Position.

Thanks for any advice.

[ritste20]

Apply a rigid joint between the component origin and the assembly origin.

This will prevent accidental movement in the future and won't ask you to perform a capture position event.

Regards,

[j9lemmon]

Thanks @ritste20 

The problem is, the body is not part of an assembly.

Is there any other way?

Or if I choose Continue when I get these messages, will the body go back to it's old, desired position?

[ritste20]

Yes clicking continue will revert the body back to it's last defined position.

But the more important question is why are your bodies not fully constrained in space to begin with if you're not working in an assembly environment?

EDIT: If you followed rule #1, you are by default working in an assembly environment... This is part of top-down modeling philosophy that Fusion was built around.

Speaking from experience, it takes a concerted effort to use a bottom-up approach in Fusion but that is how my brain was originally wired and my wife threw out the owner's manual.

[j9lemmon]

Thanks @ritste20 for this great information. The Rule #1 link was very helpful.

Re constraining a Body, I know about constraining a Sketch; but I can't say I fully constrain every sketch I create.

Is there a way to constrain a Body other than fully constraining underlying sketches?

[ritste20]

To be perfectly honest, I don't know. I always do whatever I can to fully constrain my sketches. Sometimes I think it's harder in Fusion than some other CAD programs because it doesn't show you the underconstrained degrees of freedom for the sketch geometry (at least I haven't figured out how to yet) so it can be a bit of a guessing game...

If your initial sketch is fully defined and you don't have multiple disjointed bodies within a component, then it should remain locked in position (relative to the component origin), but you still might be able to accidentally manipulate the geometry if it isn't fully constrained.

[j9lemmon]

After more reading, I'm going to follow your advice @ritste20 and create an assembly of my existing parts, then create rigid joints. All these parts are within one Master component. I figure I'll need to do these steps:

1. create a New Component name it Fin Assembly
2. drag the 3 parts, each of which is a component, into the Fin Assembly folder
3. Create a Joint using these 3 components
4. Make the Join Rigid

Is this correct, or am I missing something?

Thanks again for the great advice.

[j9lemmon]

I did the steps above, and then it looks like, in Browser, I can make the 3 components a Rigid Group by right-clicking the Assembly Component holding those 3 components, and then choose Rigid Group. 

I think I don't need to create Joints between the 3 components, because they do not move relative to each other.

Sound right?

[chrisplyler]

GROUND the component that the body is in.

[ritste20]

Yes, but I would still position it at the origin prior to grounding it...

[chrisplyler]

Oh...you didn't create it at its Origin to begin with? Any logical reason why not?

You don't really HAVE to...it's just nicer/cleaner in my opinion.

[ritste20]

Because I don't use a top-down modeling strategy. My components are always created at the origin, just in their own document.

I also generally disregard rule #1 because that's not how I do things, but that doesn't make it wrong.

[etfrench]

Use a joint to position the bodies (after making them a component) instead of moving them into position.  Moves are not parametric, so if you change something, the bodies won't move.  For example if you have two axles 5' apart, then move wheels to each axle, when you change the distance between the axles to 6', the wheels won't move to the new position. With a joint, the wheels will move to the new position.  The other big drawback to the Move command is that each and every Move command has to be recomputed every time a change is made in the file.  This can dramatically slow down the compute.

[chrisplyler]

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@ritste20 wrote:

Because I don't use a top-down modeling strategy. My components are always created at the origin, just in their own document.

I also generally disregard rule #1 because that's not how I do things, but that doesn't make it wrong.

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Soooo... if you created them at their origin... why would you have to move them to the origin before you ground them? I'm confused.

[j9lemmon]

Great advice @etfrench 

That helps my understand the value of using Joints, even if parts won't be moving relative to each other.

[j9lemmon]

Thanks @chrisplyler 

I was a complete newbie to F360 when I started designing my current product. I centered the entire product at the origin and then as I created additional parts, I positioned those parts relative to the entire model.

I realize now, I should have created a separate assembly for each collection of parts that fit together. So each assembly would have its own origin. Should each model within an assembly also have it's own origin?

Also, there was a mention of creating a part in its own document. I've been  doing the entire product in one F360 file; there have been no performance issues, because the product is not highly complex.

In my case, is there a compelling reason to create parts in separate documents? I want to follow practices that will make it easier to make changes.

[ritste20]

I was responding to your comment in regards to the OP's question. I don't use the move command. Ever.

The OP obviously is dealing with some positional issues which means whilst moving components around, there probably isn't anything situated at the origin any more. I was trying to encourage them to start from a fixed point (the assembly origin) to place the base component where it should be AND THEN ground it. Not just grounding it willy-nilly somewhere in space.

There was no context to your original post about grounding and obviously, the conversation needed some clarification.