Modeling by the interference of two bodies

[ViniciusV]

Hi,

I'm using NX 7.5 and I wonder if it is possible to shape a model by removing what may be interfering with another body.

For instance, I'm trying to design a cams, but I found out that drawing its curves would be harder than trying to do this. So what I'm planning to do is since I know every position of this cams and the rod it will actuate I thought of drawing a simple cylinder and then by rotating the two bodies I could remove the material of this cylinder which is interfering with the rod.

Please give me some tips, thanks.

 

[MickyV007]

This is called Intersect function, it is one of the Boolean function you can choose when preforming a extrude or revolve.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit (Intel(R) Xeon(R) CPU X5650 @2.67GHz)
24.0 GB
NVIDIA Quadro 4000 + NVIDIA Tesla C2050

 

[JohnRBaker]

Unless you're dealing with a very simple cam profile this may notbe very practical. That being said, there is a tool which will create solids which represent the interference between bodies which can then be used to remove the that interference using a Boolean subtact.

Go to...

Analysis -> Simple Interference...

...and in the section of the dialog titled 'Interference Check Results' set the 'Resulting Object' option to 'Interference Body'.

Note that this function will work either in a simple part model with multiple bodies or in an assembly where the Components interfer.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[ViniciusV]

Yes, I'm familiar with this tool, but I thought I could only use it while modeling one body, how can I do this in an assembly and select a different body as the body interfering with the one I'm extruding?

Or maybe I wasn't clear enough with my question.

 

[edgray]

A function that I have been wishing for for a long time is to create a solid by extruding, revolving, or sweeping a solid.

I am still stuck in NX5 so this feature may now exist for all I know.

 

[ViniciusV]

Thanks John, I'll look into it. My last reply was for Michael.

I can attach a picture of what the cam should look like. I did it before by skecthing every point of it, but that was not practial.

The attachment shows a simple model of the cam and rod. What really matters for me is the cam itself, the rod it is actuating will be different, but the cam will continue to actuate in a small cylinder in that rod, just like the picture.

But during an analysis I realized that the cam should be actuating in a different point of the rod, that is why I came up with this thread, I don't want to sketch it again.

 

[ViniciusV]

I forgot to ask how can I subtract the interference body created by the analysis with the cam durring assembly? When I select Subtract i won't let me select the cam body.

Thanks.

 

[cowski]

Export or wave link the interference body to the cam file and subtract it there.

http://www.nxjournaling.com

 

[JohnRBaker]

Set the 'Cam' Component to be the Work Part and the 'Interfernce Solid' will now be created in the same part file as the Cam.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.