NX separate motor shaft from solid body 2

[Simemg]

Hello, I have a solid body from a .step file, i am interesting on separate the motor shaft in order to have 2 solid body then i can use the motor shaft as a rigid body on mechatronics concept designer for simulation purpose (moving motor shaft, coupling and actuator), i attached some pictures I found to explain better. Thanks in advance.

 

[Ehaviv]

use split with extrude
and select the shaft face

 

[Toost]

find a feature named "Bounded plane", then select the edge shown in the attached image.
This will create a separate sheet body * inside that edge. * a surface.
Then find a feature named "Split body" , select the motor as target and the new sheet body as the tool.
this will cut the shaft from the motor housing into two solids.

You can extrude the same edge inwards into the motor , and set the resulting body , in the extrude dialog, to sheet body.
that will create a cylindrical sheet body, open in both ends, then repeat the bounded plane inside the motor, then find a feature "sew" to join the two sheets.
and again use split , this will make the shaft go into the motor housing.

Regards,
Tomas

 

[Simemg]

Thank you Tomas, let me show you the result i have:

I am wondering if i did follow exactly your instructions, also i have another question: how can i convert all operations on model history to body(1) for example?

Regards.

 

[Toost]

Body (1) is the imported solid body you started with.
I assume that this was a solid body and not a sheet body. On a solid body the exterior faces are enclosing a volume, there is logic connecting the faces such that the solid modeler "knows" that it's "watertight" , The volume can be calculated by a single click.
A sheet body might be enclosing a volume but the solid modeler regards the sheet body as open, the edges have at least one opening. the volume can only be calculated with some manual assistance.

The Unsew feature i see in your feature tree should not be needed.
If the Body(1) is a solid body, we will be creating a "knife" by the extrude and the planar surface plus the sew feature.
then that "knife" can cut the shaft from the housing. You will after that operation have three bodies, two solid bodies and one sheet body.
If you remove the parameters of the shaft, that will be renamed into "Body(3) and you can then delete the "knife".
remaining : body(1) and Body(2)

Search for "Remove feature parameters".


Regards,
Tomas

 

[jerry1423]

A tip
Before you do what is mentioned above it helps if you do an Optimize Face to the models.
Select all the faces with a rectangle when you are in the command.

Jerry J.
UGV5-NX1884

 

[Simemg]

Thank you Tomas for information and Jerry for that tip, now I understand more about what i am doing and finally get the the part as wanted.