Transforming a Body parametrically in NX3 5

[josephv]

Hello all,

Was wondering if there is a way to Transform a body in an NX3 part "parametrically"?

I have a body in a part in NX3 and then I do:

Edit > Transform...

The body moves; however, the "transformation" is not recorded in the part navigator so there is no way to "remember" what transform took place (i.e. it does not appear to be parametric).

When I transform a body in SolidWorks and CATIA a Transform feature is created. This feature can then be edited or removed. It appears that UG NX cannot do this.

Please let me know if there is a way to do this. Perhaps NX4 can do this?

Kind regards,

Joseph

 

[Xwheelguy]

The transform command in NX is NOT associative or parametric.

You will not be able to associatively transform your model until NX5 is released (using the approach you described above).

This doesn't mean there isn't some obscure workflow (like using datums or WAVE) that will allow for a transformation of some sorts, but you typically have to think ahead when you're starting your model in order to use that sort of approach. Had I the experience in doing something like that, I'd offer a suggestion, but at the moment I'm drawing blanks.

I know, it doesn't make sense why mid-range modelers and other high end softwares like Catia or I-deas might be able to transform associatively, but UGS has seen the light and it's coming soon....already have seen it in action and it's pretty nice.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[JohnRBaker]

First, I would be careful with what you may think is coming in NX 5. What we're adding in NX 5 is something called "Geometry Instance" and what it will allow you to do is perform a 'parametric' Tranform-Copy. In fact, as many 'copies' as you wish, unless your wish is to only have ONE, the original body, just in a different location (of course, you could always make a copy and then 'Hide' the original)

However, that being said, there already is a way to do what it appears that you want in NX, and it's been there for years (well, at least as far back as UG V18.0) and it does NOT require any special planning nor the creation of reference objects, or anything like that. Just go into Insert/Direct Modeling/Move Region... and when it asks you to select a 'Seed' face, just select ALL the faces of the body. You can then skip the second step and go directly to defining how you want to move the 'body' and enter the desired parameters and hit OK. Granted, for compound moves, like in both an X and Y direction, you'll need to do this twice, but you will get a set of expressions that can be edited to control the location of the solid/sheet body.

Now if you'r running NX 3 or NX 4 AND you're willing to create AT LEAST ONE point ahead of time, you could create a 'Smart Point' and using the above approach perform a 'Point to Point' move selecting some vertex of your body as the 'From Point' and the Smart Point as the 'To Point'. Now you will have full X, Y, Z control of the location of the Smart Point and if you move it the body will move with it.

And this leaves no 'copies' behind since it acts like a true 'Transform - MOVE'.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

 

[Shadowspawn]

John,
Is there any way to do this with linked curves from a component in NX3?

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[Xwheelguy]

For clarification, I was confusing Geometry Instance with Transformation. Geometry Instance will be coming in NX5, while Tranform is supposed to be overhauled in the near future (based on discussions with a development manager).

Just wanted to clarify that I'm not "thinking" anything is coming in NX5...I just got my wires crossed a little. My apologies. Never fear though...John will be sure to set the record straight, obviously.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Shadowspawn]

John,
After a couple of cups of coffee and re-reading my question, a little more background info would help... So without too much fodder, what I'm looking for is a way to simplify the current process...
I'm a die designer for turbine airfoil blades. I take the finished airfoil definition from the customer and design dies to forge steel into the desired shape. There are a number of section cuts, taken at various heights of the Z-axis of the blade, to give us 4 splines representing the convex, concave, leading and trailing edges of the blade at those sections. The legacy method involves using various grip routines to add the required pre-corrections to these curves (read no associativity via a series of transform/copy of the original curves at each section height...).
I'm trying to develop a process where the pre-corrections are associative. So far I have a template file created to get all the necessary section curves at the prescrived heights, and these are linked into a separate part.
I'm then taking these curves, generating a ruled surface between the convex and concave airfoils, and then adding all the pre-corrections necessary with a series of arrays (grouped feature) of the ruled surfaces. I'm then using the edges of the surfaces to extract curves and attach a series of sketches for the flashing. This does seem to get us what we need, but the process can be simpler... or so it would seem (updating can get hairy and there are unwanted surfaces generated from the patterning).
Thus, I was thinking that one of your suggestions might be a better approach. The pre-corrections involve dance of multiple X and Y translations, XY rotations, and offsets. Any thoughts and suggestions would of course be appreciated...

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[JohnRBaker]

Without writing special NX Open and/or KF code, I don't think you can do what you want in NX 4. However, Geometry Instance in NX 5 sounds like it might help you with your current workflow, but of course, NX 5 is still 5 or 6 months away, but at least we're working on adding more functionality like this.

Sorry, I couldn't be of more help.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

 

[mjcole]

John,

Good Tip, I started writing mine then scrolled up and saw that you mentioned the moved region option which I showed a co-worker could be used to keep a Block feature continuously centered on the Origin using this option but it did require 3 features.

Are you working on unlimited undo redo for features which I saw in the NX users survey?

Michael

 

[JohnRBaker]

Are you working on unlimited undo redo for features which I saw in the NX users survey?

I'm not sure that I would use the term 'unlimited', but we're getting pretty close. For NX 5, Redo will be available for all feature creation and editing operations that have been updated to the new User Interface standard (perhaps 80%-90% coverage for modeling, perhaps a little less coverage in Drafting and while it appears that CAM will also have good coverage, we're not really sure what 'Redo' will actually mean in that kind of environement).

Anyway, NX 5 should go a long way in addressing this expressed need for a general purpose 'Redo' capability in NX.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

 

[josephv]

Thank you everyone for your tips.

And thank you, John, we tried Insert/Direct Modeling/Move Region... and it works great.

Is there any way we can avoid selecting ALL the faces of the body? Or instead... is there a quick way of selecting all the faces in a body (e.g. selection filter command)?

Kind regards,

Joseph

 

[JohnRBaker]

Is there any way we can avoid selecting ALL the faces of the body? Or instead... is there a quick way of selecting all the faces in a body (e.g. selection filter command)?

Not at this time. For NX 5, 'Direct Modeling' is not one of the areas that has yet been given the full NX 5 User Interface update treatment so there are no changes there yet. However, I suspect that in the next go around we may see some improvements there including using the general 'Selection Intent' scheme, which would provide more selection methods including selecting all faces of a body.

But that being said, by that time I fully expect that we will have, for all intents and purposes, replaced Tranform with functions that will perform BOTH parametric 'Copies' AND 'Moves', which would make the use of 'Move Face' for this purpose completely unecesssary.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

 

[Xwheelguy]

Yep...that's what I've been hearing from UGS development during PLM World meetings. Transform is due to be overhauled to allow for associative transformations, rotations, etc. This MIGHT be on the plate for NX6. We haven't discussed it too much since we're still working on NX5 projects (Geometry Instance, Feature Arrays, 3 Faced Blend and Holes in Non-Planar faces). Note that the last 2 are looking very iffy.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[josephv]

Thanks again for all your tips.

The Direct Modeling, Move Region works great. And you can select all the faces by just doing a window drag on a body while running this command.

We would like to automate this a bit.

Is there a Move Region (or a parametric move) available in the UG API(C++ or GRIP)?

Thank you all once again,

Joseph

 

[DavidTolsma]

I would hope that some NX version in the near future that they put drag handles on all objects, like assemblies have. This would eliminate the Transform dialog that has been with us since at least V10 days. Add a context menu to do the instances and we are all set.

-Dave
PLM Exchange

http://plmexchange.net

http://groups-beta.google.com/group/NX_CAX/

 

[dcadcam]

Hi,

It is possible to transform anny body parametrically in NX3.

First you have to group this body (RMB - Group).
Then This Groupfeature behaves its self like a normal feature and with Instance you can transform it parametrically.

Kind Regards.
Erik van Diepenbeek
CAD CAM designer
Sealedair - Venray - the Netherlands

 

[DavidTolsma]

dcadcam, thanks for the tip. I will have to give this a try.

-Dave
PLM Exchange

http://plmexchange.net

http://groups-beta.google.com/group/NX_CAX/

 

[Xwheelguy]

dcadcam,

You cannot transform a sheet body that has been trimmed in NX using Group Feature, so not just any body can be transformed parametrically.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com