A move that is not useless?

[Anonymous]

Is there a way to move an object fully? I used the "move" tool from the 3d model toolbar and the solid looks like it has moved. The thing is when i try to do anything with it (in this case make a circular pattern) it gets completely unclickable. I can still make a pattern out of the original outlines for the solid, but not for the moved part.

If anyone knows, why is this even a feature? To only half-move a solid, not actually moving its root. 

My solid is a loft, made from 2 perpendicular 2D sketches.

(Inventor is in my opinion completely unbearable when it comes to simple things like constraining to reference points and moving parts.)

[JDMather]

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@Anonymous wrote:
...(Inventor is in my opinion completely unbearable when it comes to simple things like constraining to reference points and moving parts.)

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Can you attach your *.ipt file here?

How much training have you had using Inventor?  (I must admit that I don't understand why you would want to "move" a part.)

[Anonymous]

Ok, here you go, thanks fro quick reply!

[blair · Accepted solution]

I don't think you understand Inventor, as JD's post. You need a new IPT for part and then you place them in a IAM assembly file. Using the Constraints to position and mate the parts together to form your assembly.

The only time the Move command is used within a IPT part file to either relocate or reorient the part with respect to the Origin. 

Some NC tool path software requires the plan view of a part be in the XY plane. This is the only time I use the Move command.

[blair · Accepted solution]

Looking at your file, the Ring (Extrusion5) should be it's own IPT file and the curved Fin (Loft2) should be it's own IPT file. You would then create a new IAM file and place the Ring first and ground it. Then Place the Fin in the IAM file and use the Constraint Commands to locate and mate the Fin to it's correct position. 

Then use the Array command to pattern the file around the Ring.

You don't have any dimension on your Ring, the green lines in the Sketch4 will turn black when they are fully dimensioned. The same can be said for your Sketch3 within the Loft.

All these items should have been covered in your training as they are basic concepts. 

[blair · Accepted solution]

You should also post which version of Inventor you are on.

[JDMather · Accepted solution]

Can you attach an image or link of what you are attempting to model?

Is there a reason you used a Zero dimension in Sketch1 rather than a Coincident constraint?

You don't necessarily need to do this in assembly - you can probably use multi-body and then push out the assembly, but I would need to know your Design Intent to make that determination.

Sketch3 does not have any dimensions?

How will they know how to manufacture this without dimensions?

Sketch4 is not fully defined?

WorkAxis4 is an unnecessary duplication of the Y axis?

Is something like this what you are after?

[Anonymous]

Inventor professional 2018, if that helps, don't know how to check more
specific details though, sorry.

[Anonymous]

The underconstrained sketches was purely for testing purposes only, i do not intend to manufacture this part, im only interseted in learning inventor cadding since it has propper analytics software, unlike its free counterparts.

[WHolzwarth]

Hmm. That's strange. Is anyone else getting an error, when trying to move the first solid?

I do.

[JDMather]

No errors here.

[WHolzwarth]

That's going on with German Inventor 2018. (Mp4 in zip)

I'll try it again with ENU version.

[WHolzwarth]

Same in ENU version. Here's the file (2018 IPT)

[Anonymous]

Thanks everybody, for now i kinda know how to do it :). Now could someone explain to me what this feature is good for in contrast to just moving in a single flie? Just curious.

[JDMather]

How much training/experience do you have with Inventor?

I ask, because it is still unclear to me exactly what you want to accomplish.

Do you have an image or link to something similar to what you are trying to design?

In the following, I am going to assume that you have zero training/experience.

In Inventor you normally work as though you are making physical parts and physical sub-assemblies and assemblies.

That is, one part is one file.

One sub-assembly is a collection of parts put together by certain rules (Constraints limiting Degrees of Freedom).

On assembly is a collection of parts or sub-assemblies or parts and sub-assemblies (just like the real world).

My guess is that you are trying to model all of your parts in on part file, which can be done, but isn't a logical representation of the real world.

If you want to get the physical dynamics of real world assemblies - you will want to learn to follow real-world logic in the design of your parts, sub-assemblies and assemblies.

Once you gain experience, then you can "cheat" in the digital world with techniques like multi-body solids.

But for now, you should stick to duplication of the real world in your virtual design world.  

1part=1file

As such, there is seldom a need to move a part (or feature) within a part.

Now this can by used in some powerful modeling techniques, but probably not for a beginner.

You move parts in an assembly (space), not in a part.  

Logically moving a part in a part doesn't even make sense in the real world.  I can't even think of an example where that is possible.  Maybe a deformation forming process could be considered "moving a part in a part".

[JDMather]

Walter, I didn't look at your video before.

I did not use the Direct Edit, I used Move Bodies.

When I use Direct Edit>Move Solid - I do get the error.

So I created a new file with two bodies and tried in the new file and I do not get an error, it worked as expected.

I do not know what it is about the Thing file that is causing the error.

[WHolzwarth]

Interesting, Jeffrey.

Looks like some task for Johnson @Anonymous

[JDMather]

I thought maybe it was because of the offset workplane used for the Loft sketch.

But I just created a new part file with a Loft and I could use Direct Edit > Move Solids without any issue.

There is something specific in that "Thing.ipt" file.