NX questions 1

[bartbrejcha]

Is there something I'm missing with the interface to allow insert mode like in Pro/E or Solidworks? In Pro/E I want to drag the red arrow up so when I add a feature it stays where I insert it. The work around which Is what I would teach is to add the feature at the end and reorder the feature to the appropriate location in the model tree.

I have a problem re-associating first part in assembly. I can simply rebuild the assembly but I want to fix the one I have. How can I redefine the first component of the assembly to reference the coordinate system instead of just placed in there twisted.

How do I show the dimensions in a drawing that I used to create the part? I know how to create new dimensions.

Is there a top down modeling methodology like in Pro/E 'external copy geometry' or in Solidworks 'insert part'

how can I select an edge w/o roaring the model? is there a Query function?

 

[JohnRBaker]

OK, let's take these one at a time (in the future, it may be better to start a different thread for each topic/question and also, please indicate which version of NX are your questions being asked in reference to):

"Is there something I'm missing with the interface to allow insert mode like in Pro/E or Solidworks?"

If you wish to insert a new feature somewhere back in the parts 'history' go to the Part Navigator and while in 'Timestamp Mode', select the feature that you would like the new feature to be created after, press MB3, and choose the 'Maker Current Feature' option. This will roll the model back to where the feature that you selected is the last ACTIVE feature and you can now add any new features that you wish and once completed, just go back to the Part Navigator and select the LAST feature on the on the list (it willbe grayed-out but that's OK), once again press MB3 and select the 'Make Current Feature' option.

There another way that you can do this as well, and that is to use the VCR-like controls found on the 'Feature Replay' toolbar to 'rewind' your model to a certain point or start at the very beginning and then 'jog' the model forward using the 'Make Next Feature Current' button (►|)until you reach the point where you wish to insert your next feature. Once that's done you can continue to 'jog' forward one feature at a time or you could hit the 'Make Last Feature Current' button (►►|) which will take you back to your completed model, just with the new feature(s) inserted where you wanted them.

"I have a problem re-associating first part in assembly. I can simply rebuild the assembly but I want to fix the one I have. How can I redefine the first component of the assembly to reference the coordinate system instead of just placed in there twisted."

Not sure exactly what you're driving at here, but there should be no problem placing any component anywhere in the so-called assembly structure and then constraining it to be fixed and having other components than constrained relative to it, at least NOT since NX 7.5 when Mating Conditions were completely replaced with Assembly Constraints.

"How do I show the dimensions in a drawing that I used to create the part?"

I assume that you mean the Dimensions that you created in a Sketch that was used to create a part, correct?

Well once you've got the Drawing views placed, go to...

Insert -> Dimensions -> Feature Parameters...

...where you will be able to drill down to the particular sketch of interest, select it and indicate which views you wish to see the dimensions in.

"Is there a top down modeling methodology like in Pro/E 'external copy geometry' or in Solidworks 'insert part'"

I think you need to look at the NX Help file for the section covering the WAVE functionality and see if this is what your looking for.

"how can I select an edge w/o roaring the model?"

First I'm assuming that you're talking about w/o "rotating" the model, correct? If your question is because you're working in a shaded display but you would like to be able to pick THRU your model to some edge on the back, yes there is an option that you can toggle ON/OFF in the so-called 'Selection Bar' which controls this behavior, as shown below:

Anyway, i hope this helps.

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.

 

[bartbrejcha]

John. Awesome!

For the First part in the assembly... I am having problems re organizing it in 8.5 to look instead at the coordinate system. It's rotated slightly and when I create a drawing of the assembly the template has it rotated slightly the same as in the assembly... otherwise I wouldn't care so much. I did rebuild the assembly but I would like to go back and fix the original assembly.

A workflow that works well with me in SW or Creo... Ill make a detail drawing of the assembly and dimension interference and clearance issues that will need modifying. Ill change a part by the around of interference/clearance and update the drawing to see the dimension update to zero. When I try this same workflow with NX I can't seam to edit the part until I exit from the drawing. Is there a way to change the gateway maybe to and from part and drawing efficiently?

I scaled a model at about feature #10 and it worked just fine. I had mm and inches mixed up. But when I go back to before the scale (its a feature) the part is still in millimeters. I'm I to understand that's how it's done or maybe there is another way to scale or maybe I should have remodeled the part once I realized I was doing one inch = one mm ??

 

[JohnRBaker]

See, this is where it's going to get hard to respond since we've got multiple questions again.

Anyway, for your Assembly issue, make sure that you have a Datum CSYS in your Component part as well as your Assembly. Add the Component wherever you wish using the 'Entire Part' Reference Set and then select...

Assemblies -> Component Positioning -> Move Component...

...and then select the Component that you wish to move and in the Transform section of the dialog set the 'Motion' option to 'CSYS to CSYS' and then simply select the CSYS in the Component and then the CSYS in the assembly. Once it's been moved you can then assign it an Assembly Constraint of 'Fixed' so that it will remain where you placed it.

We do not recommend that you try editing the Model while in Drafting. It's just a poor practice.

How is it that you think you've entered an Imperial value in a Metric part? But this you need to be aware of, once you create a new Part in NX, there is NO easy way to change the base units of measure. Metric parts remain millimeter units and Imperial parts remain inch units. So unless you did something special (and there ARE ways to do this), when you add a new feature to an NX model the input units will match those of the part file.

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.

 

[looslib]

Changing a part's units from imperial to metric is not as easy in NX as it is in Pro/E.
Pro/E - Setup - Units and select the new units then determine if you want the same size (1"=25.4mm) or same dimension (1"=1mm).
NX you need to use a supplied utility program that will change the part file base units (ug_Convert_part.exe). This can be run in batch mode.
Prior to NX6(?) it always did a scale conversion (1"=1mm) but with the addition of parametric units of measure, I think it now does a same size conversion. (John can correct me)


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

The conversion utility is still available but it should only be used if you truly need a part file in a specific base units, either millimeters (Metric) or inches (Imperial). Howevet, if you wish to insert a feature based on different units than the base units there are other less drastic approaches that are available. For example, if you wish to insert an ANSI standard clearance hole or threaded hole into a Metric part file, that can be done directly inside the Hole Feature dialog by selecting the appropriate standard. Also, the Expression system allows you to select whatever units are appropriate for the dimensionality of the expression being created and while you can't change the units of an expression created when a feature is added to the model, you can use secondary expressions to convert from one set of units to another as long as you don't violate the dimensionality of the original Expression (example: You can't use millimeters to define an angle, or inches^2 for a volume).

But the one that is probably most useful, and leat understood, is the option to TEMPORARILY switching the input (and and output) units for Modeling when creating features and such. For example, by using this option, I could have a Metric part file where when I create a Blend, I'm asked, in the Blend dialog, to enter a Radius value in Inches.

To temporarily (for the duration of the session) change the units that the system is working in, go to...

Analysis -> Units <current part units> ->

...where you can either select a different standard based on an appropriate 'Mass - Linear' convention or where you could define a totally custom set using the tools found under this menu item. Note that changing the units while working in a Metric part from the default 'kg - mm' to say 'lbm - in' does NOT actually change the base units of the part file, but rather will simply switch all of the feature dialogs to using Imperial units, in this case Inches for linear inputs. It will also switch the units used when doing a measurement function, like Distance or Mass Properties. Once a part file is saved and reopened it will revert back to the default input units as per the base units of the part file.

Anyway, I hope this helps you understand how NX handles working in different units or standards.

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.

 

[deedub777]

Other ways to 'make current feature' is using hot keys to step through the part navigator:

Ctrl+Shift+Home - make first feature = current feature
Ctrl+Shift+Left arrow - make previous feature = current feature
Ctrl+Shift+Right arrow - make next feature = current feature
Ctrl+Shift+End - make last feature = current feature

I usually use the RMB method to insert a feature and then Ctrl+Shift+End to roll right back to the end.