Move a derived part

[shastu]

How do I move a dirived part to the center of the origin?

[R.Corriveau]

I don't think you can.
You could try to create a new asssembly and constrain the part to the origin then derive again.

[Anonymous]

What you could do is locate the original in an assembly at the origin and then derive the assembly into a new part.

[Anonymous]

You could open the base component and edit the very first feature in the
part. Then constrain the sketch to origin.

Johnson Shiue
Test Engineer
Autodesk, Inc.
wrote in message news:4995435@discussion.autodesk.com...
How do I move a dirived part to the center of the origin?

[shastu]

No, actually I can't because the link was broken from the base component.

[Anonymous]

In that case, place the derived part in an assembly, constrain it to the
origin the way you'd like, derive that assembly into an .ipt, break that
link.

Patrick

[Chassuer]

You can actually move a part that you derive into an .IPT. Its the Move bodies command. It is on the 3D Model tab under modify and you have to click on the down arrow to access it. Once you click it you will be asked to click on the body you want to move and then you can move it based on the X, Y, or Z and there is also an option to free drag it or rotate the part. Hope this helps

[JDMather]

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@Chassuer wrote:

.... Its the Move bodies command. It is on the 3D Model tab ...

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@Chassuer

Did this Move Bodies command exist 12 years ago?

Did "tabs" exist 12 yrs ago?

[iMaJiNe_Designs]

Is there any way to have a sketch move with the body using the 'MOVE BODIES' command on a derived part?

[johnsonshiue]

Hi! The derived sketch cannot be moved. If you want to move the derive part in the model space, you may want to consider using derive assembly instead. Basically, you create a new assembly and insert the source part. Then you derive the assembly as a part. In Derive Assembly dialog -> go to Other tab and select the sketch to derive. If you want to relocate the sketch, simply open the source assembly and move the source part to the desirable place. The derive assembly part will update accordingly. Please let me know if you have any question.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2015...

Many thanks!

[iMaJiNe_Designs]

Thank you for the reply Johnson.  It just seems odd to me that the sketch of a derived part doesn't move with the body.

[johnsonshiue]

Hi! This has something do with how Inventor derives the objects. The sketch and the solid body are both derived from the source part. In the derive part, the derived sketch and the derived body are like a clone of the source geometry. When you move the cloned body, the clone sketch isn't aware of the move because it is dependent on the source sketch (and source body), not the clone body.

Unfortunately, there isn't a command to move a derived sketch. It is always located at the same place as the source sketch. You can add or remove geometry from the derived sketch though.

Many thanks!

[sschulteH6WZ3]

All you get with that is crude movements there is no way that I see to precisely place it.

[JDMather]

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@sschulteH6WZ3 wrote:

All you get with that is crude movements there is no way that I see to precisely place it.

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@sschulteH6WZ3 

Isn't this a duplicate thread?  Wait a minute - this thread is 16 years old?  The tools have changed.

Snap to precise location.

[johnsonshiue]

Hi! Did you try Direct Edit command to relocate the solid body?

Many thanks!

[brad.wolfgang]

Hi everyone. Apologies if I am out of line here. This is my first post to the Autodesk Forums.

I often use pretty much all of the available entities and features - eg bodies as solids or surfaces, sketches, work planes, axes & points - from multiple Derived parts and assemblies as reference geometry into a new, often multibody, part being created.

Unfortunately, as soon as you use the Move Body command (whether precisely or not!) on just a body from a Derive, it negates any use of the rest of its derived work features and geometry, as they are now out of position with respect to the derived body. As mentioned above, it does not seem possible to also move the work features.

The problem discussed here arises when the entities of the derived part/assembly do not happen to be in the position you want them in the new part when the origins of the new and derived parts are matched. PLEASE PLEASE correct me if I am wrong, but unfortunately there is no availability to align and lock any feature within a derived part/assembly to any feature of the new part to position the derived part - except of course for the default of matching the origins of the derived part/assembly and the new part.

The old add-in called DerivedPart_SP attempts to address this by allowing the derived part origin to be matched to the coordinate system of a sketch within the new part. At least then you can use enough construction to get the sketch coordinate system in the right place for the derived features to be where you want! The big failure of DerivedPart_SP is that you only get one shot at positioning the derive when the add-in is run and unfortunately the origin of the derive does not remain associatively linked to the coordinate system of the sketch. As soon as you make any changes to the model, the derive will likely be out of position again - with no way to fix it. 😞

I never got around to trying DerivedPart_SP on a derived assembly, so I don't know if that even works. I had already given up in disgust using it on derived parts before I learned how to use derived assemblies.

Using a dummy assembly to reposition a part or assembly before you derive it into the new part is only a bit better in that, while you can later re-position the derived part within the dummy assembly and hence your new part, you still can't tie it back to geometry of your new part. Inventor spits a cyclic reference error when you try to insert your new part as a positioning reference back into the dummy assembly.

Is there any way to ask the Inventor Developers to, on the dialogue windows for Derived Part and Options tab for Derived Assembly, also include an option to associatively tie the derive origin or other UCS to a UCS or sketch coordinate system somewhere in the new part? There are already options in the dialogue windows to scale & mirror it!

Solid Edge had this functionality available in the early 2000's in their Part Copy command. (I'm not pushing Solid Edge - they are a pack of b's - but that is another story...)

With regard to the cyclic reference error, it would be good if the checking for this problem was not done until after a part is inserted and then edited. At least then you should be able to avoid using the actual features in the part or assembly that cause the cyclic error and still use other features that don't.

Apologies for the length....

[brad.wolfgang]

I'd recommend the addition in the dialogue windows for Derived Part and Options tab for Derived Assembly should be just a single line in each, located immediately above the "Scale factor" & "Mirror part" or "Mirror assembly" setting boxes.

The line would be titled "Derived part position" or "Derived assembly position" or similar as appropriate.

The line would contain two drop-down selection boxes. The first one labelled "This part position from", the second labelled "Derived part(or assembly) position to" or similar.

Each of the drop-down boxes should allow selection of any of the origin, all UCS's and all sketches available in its respective model. I'm not sure if any other Inventor features have coordinate systems defined, but if there are any, they should be available for selection here too.

The default population of the two positioning boxes should always be Origin / Origin. This way, the addition would be unnoticeable to anyone who did not want to use it, and should make it backward compatible with earlier Inventor versions.

[johnsonshiue]

Hi Brad,

If I understand your request correctly, you would like to be able to derive a part or an assembly by relocating its origin. There is indeed no workflow to do that in Inventor. Relocating a part entirely (including the construction geometry) has to be done in an assembly. The dummy assembly workflow you mention is the workaround. I am wondering if defining a UCS can help a bit. UCS is a user-defined coordinate system. You may add it in a part or an assembly. Then you can constrain two UCS' in the dummy assembly more easily (Relationship -> Constraint Set).

Many thanks!

[cadman777]

Hey Johnson,

Recently I started a thread that asked how to replace a model base view in a drawing so that the new base view part will orient correctly. We arrived at the conclusion that the part's orientation is based on and fixed by the world origin axes. The conclusion was, there is no way to change the orientation of a part in a drawing view. So, are you saying that is possible if the UCS is changed in the art or assembly? During the experiments I did for that thread, the option of using the UCS to achieve that wasn't tried. I can't imagine that it would work since the part's orientation and position are fixed by the world coordinates origin. What do you know about this?

[brad.wolfgang]

Thanks for the quick reply Johnson!

I would ultimately like to be able to:

1. Create a new part. (for simple example, a pipe)
2. Build enough of the new part's tree of work features & bodies to define the required position for features from an external reference part into it. (eg know within the model where and what orientation the end of the first section of the pipe is)
3. Derive an external part, locked associatively into position onto the geometry already in the tree. The derived part's sketches & work features need to remain in the correct location around the derived part. (eg put a flange in the correct position on the end of the first pipe & use a sketch in the flange part to check for required clearance in the new part.)
4. Create more geometry & work features in the original new part's tree. (eg another pipe leading from the last flange.)
5. Insert a different derived external part or assembly into yet another position on the new part. (eg, a valve assembly onto the end of the second section of pipe. This time perhaps use sketches, surfaces, a work plane & multiple bodies in the valve assembly to confirm adjacent clearance.)
6. And so on for as many derives as are required, each with its origin in a different position in the new part.
7. Be able to edit the first pipe and have all of the derives automatically move to their new positions within the new part.

Please be aware the pipe & flanges are just examples. I am actually modelling more complicated assembled parts around reference model assemblies that can contain hundreds of parts. From this work, I am now pretty good at manipulating derived assemblies to display only parts & features I need.