Parametric transform

[Tisho]

Hello,

I have a "dead" non-parametric geometry, which position I want to parametrize whenever some other object(Sketches, lines, datums etc.) changes position. I want to that in a single part.
In general I am taking dead objects and putting them in model that needs to be parametrized. Thus the dead object need to move as well.
How do I do that? Transform operation is not bounded by other objects' position.
Please, advise.

I am working in NX4.

Greetings,
Tish

 

[jerry1423]

What you can do is use Move Face in syncronous modeling and select all the faces of that body.
I think that will do what you want, and it will be parametric.

 

[jerry1423]

sorry, I just saw that you are on NX4
my above response does not apply

 

[joycejo]

Could you add them as components and mate themn to the sketch and datums. When you update the sketch the components should move.

John Joyce
N.C. Programming Supervisor
Barnes Aerospace, Windsor CT
NX6.0.5.3

 

[Tisho]

@joycejo. No I can't. This is a single part-a box lets say. Dead bodies are transferred from other parts(screw domes etc.).They don't need to be parameteric but need to be carried over. I want those parts to take a new position when the box size is changed let's say.

 

[jerry1423]

I think the best you can do is have the dead geometry stay stationary and everything else linked to it.

 

[JohnRBaker]

Even though NX 4.0 does not have all of the Synchronous Modeling tools, it does support the precursor to Synchronous which was called 'Direct Modeling' and by go to...

Insert -> Direct Modeling -> Constrain Face...

...you can basically do what Jerry suggested earlier.

First choose the type of relationship (Constraint Type) that you looking for and then you select a 'Seed Face' as your first selection . When you're asked to 'select boundary faces' simply select the rest of the model using area select. Now skip the next step (whether there are blends or not is irrelevant in this case) and then select the face on the body you're constraining that you wish to constrain relative to the face on the body which you wish it to be associated to based on the type of relationship (constraint) that you initially picked.

Once established, these constraints will cause the first body to move whenever the second one is moved or the size is changed due to it being edited and the faces which were referenced are moved. If you're creative you can emulate many of what are now called Synchronous Modeling techniques only you don't have the better interface nor the smart selection.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Tisho]

Thanx John,

Constraining the face does the job. Just for the record I have a second solution.The command is called geometry instance. If you constrain the end point of a line with the parametrized object, you can use this end point as a reference for the Geometry instance command. Of course the initial object(the container) needs to be sent in a hidden layer and its instance to be used instead.
Once again, thanx for the good discussion .
Tish

 

[JohnRBaker]

Are you sure you're running NX 4.0? I ask because 'Instance Geometry' was NOT introduced until NX 5.0.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Tisho]

Yeap,

Help->about

NX Version: 4.0.4.2

Tish

 

[JohnRBaker]

Again, I don't understand your claim that Instance Geometry is available in NX 4.0. This function was not introduced until NX 5.0. Could you please point out exactly on which menu/toolbar that you found this function?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Tisho]

Here is a screenshot of my NX. This is getting interesting. I remember trying to show this command to some other colleagues of mine but couldn't find it on their environment and menus. Maybe I need to ask our CAD administrator to spread some light on the topic .
Tish

 

[Tisho]

Hm, first upload attempt has failed. Here is the pic once again.

 

[JohnRBaker]

Well, that's a new one on me...

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Toost]

An environment variable that activates this feature in NX4 as a pre-release-trial-option ?

 

[JohnRBaker]

Toost, that's what I suspect, but I don't think it was ever intended for 'public consumption', probably part of some 'alpha testing' effort prior to going into 'production' with NX 5.0.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Tisho]

Yes,it could be in testing phase. Just to satisfy my curiosity, I remember putting 0 copies in the dialog box, and every time NX was crashing with the sweet message:

Fatal error detected, unable to continue.

I am happy to know that I can crash NX everytime I want. This gives me some advantage in the modern computer world. I can still crash them not they me.
In reality the job needs to be done and there is no place for having this sort of fun

Tish

 

[JohnRBaker]

You would be much better off simply upgrading to the current version...

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Tisho]

Yes John,

The upgrade is planned for the end of the year.

Tish