make a part independent from base component

[Anonymous]

I often use a project geometry from a part I have, and create a sketch and an extrusion from the sketch and make a new body. Now I take this second solid body and I use "make part" so that it becomes a self standing part. How can I then play with this new part and modify the sketch and add things (holes, anything) to it? In the new ipt file I created I cannot see the sketch, whether I break the link or I don't does not matter.

Essentially what I would like to do is to use a part A.ipt I have to "help me" create a sketch (by project geometry), extrude this sketch and make a new solid but then save this as a new B.ipt part and use it as an independent thing, modify it etc. and delete the solid body in the original A.ipt file and have no connection whatsoever between the two anymore. I guess it is certainly possible but how?

[jtylerbc · Accepted solution]

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@Anonymous wrote:

 In the new ipt file I created I cannot see the sketch, whether I break the link or I don't does not matter.

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That's because the sketch does not exist in the second part.  It exists in the first part.

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@Anonymous wrote:

Essentially what I would like to do is to use a part A.ipt I have to "help me" create a sketch (by project geometry), extrude this sketch and make a new solid but then save this as a new B.ipt part and use it as an independent thing, modify it etc. and delete the solid body in the original A.ipt file and have no connection whatsoever between the two anymore. I guess it is certainly possible but how?

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No, you can't exactly do that.  That is not really the way multibody modeling is intended to be used.  The entire point of the technique is to have a "master" or "layout" part that centrally controls the individual parts.  Separating them afterward like you describe defeats the main purpose of this modeling technique, so it isn't an option that is provided.

Breaking the link severs the connection between Part A and Part B.  With the link broken, Part B stops updating to changes from Part A, but does not become a completely independent part with its own complete model history.  Instead, it becomes a dumb solid, similar to if it had been imported as a STEP file, with the geometry it had at the moment the link was broken.

You might consider posting some sample files, or at least screenshots, of a simple case similar to what you are trying to model.  You might get some suggestions for methods that would suit your needs better.

[johnsonshiue]

Hi! I think I know what you are trying to do. Let me first explain Make Components command. It is an important part of the multi-solid body workflow. You create a multi-solid body part whose geometry represents an assembly. In the MSB part, you can easily establish spatial relationship and geometric dependency. Each solid body represents a part.

After you are done, you use Make Components command to push bodies out as individual parts in an assembly.
For your case, this workflow may not apply. You can simply save the part as a different part file. Then you can edit the new part or the old part without any dependency.

Many thanks!

[Anonymous]

thank you. what you say at the end of your message (You can simply save the part as a different part file. Then you can edit the new part or the old part without any dependency.) is exactly what I am not able to do. Say I have a part with a geometry I want to use, a circle with four holes. I project this geometry and I create my second solid, I make a disk with that size and my four holes. Now I save it with "make part" and I call it disk.ipt. but now maybe I want to add a couple more holes to it, or do something else. and especially, I may not want it anymore in my original part, I was just using the original part because I needed its geometry (the circle and the location of the four holes) but now that part does not need my disk, I need my disk in 10 other parts and assemblies. It looks like my only solution is to break the link but then that part will become a sort of step file and all I add or delete will have to be done with new sketches, because the original sketch is invisible. right?

[johnsonshiue]

Hi! I could be misunderstanding your workflow and intent. One thing I want to add is the command called Delete Face. You can save the current part as a new part. But, you don't want the geometry which the new body depends on, right? Use Delete Face -> Lump selection -> delete the unwanted geometry. Would it work for you?

Many thanks!

[Anonymous]

hi, I was more looking into preserving that geometry, but then being able to work on it in the new part and modify it without having any connection with the original part anymore. but it looks like it is not possible.

[johnsonshiue]

Hi! I am sorry I am confused now. What you are looking for should be doable. Could you share an example of what you are doing and trying to do?

Many thanks!

[Anonymous]

  hi

how would you like me to share it?

I guess both you and jtylerbc did already answer. what I would like to do is to use a project geometry from some part and create a sketch, but then have the possibility in the future to play with that sketch and modify it, in a different place, not in the original part. In fact I may want not need at all the sketch in the original part anymore, I just used the original part for projecting a geometry and helping me to get that sketch as a starting point, but then I would like to change it in some other place and say goodbye to that original part. It looks like it's not an option.

[johnsonshiue]

Hi! If you want, you can share the ipt file here. Forum experts can take a look and provide some guidance.

Many thanks!

[jtylerbc]

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@Anonymous wrote:

thank you. what you say at the end of your message (You can simply save the part as a different part file. Then you can edit the new part or the old part without any dependency.) is exactly what I am not able to do.

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Yes you can.

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@Anonymous wrote:

Now I save it with "make part" and I call it disk.ipt.

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That's the problem.@johnsonshiue didn't say to use "Make Part", he said to use "Save As", so that you make a separate copy of the part under a new name.  You could also copy the file in Windows and then rename it.

[Anonymous]

hi

I attach here a simple example. I have some part made of three solids. for solid3 (called "newpart" there, colored blue) I used some geometry present in solid1, and I made an extrusion (extrusion6). Now, I would like to have the sketch I used for this "newpart" (sketch8) available outside this file, and modify it, make it bigger, add holes, add other things because maybe for another application I want something similar but not quite the same. The problem is if I use "make part" the solid becomes a "dull solid" as someone else wrote above, the sketch is not visible and therefore even less modifiable.

    thank you

[jtylerbc]

As already stated (twice, Post #3 and #10), the Make Parts or Make Components commands do not do what you are asking for.  The closest you will get to what you want is just saving a copy of the multisolid file under a new name, so that the new one is independent from the original.

In a situation like what you describe, I would probably not be using a multisolid technique.  I would just draw the "newpart" as its own separate part, then copy the file as needed to be able to resize, add/remove holes, etc.   If it was something I did often enough, I would consider making a template file for it so I wouldn't need to keep copying the files over and over.

[Anonymous]

hi, yes I just found out I can start from an assembly and use the project geometry from the assembly. then in the new part I just have to get rid of the adaptivity and remove the locking constraints and then I can modify the sketches. thanks!