Top 5 Fundamental NX CAD Topics You Should Know

Top 5 Fundamental CAD Topics You Should Know

So you think you don’t need NX training, eh?

In this article, we take a look at a “top 5 list” of fundamental NX CAD topics we’re betting you aren’t so well versed:

  1. Utilities Group in the Top Border Bar
  2. Details panel of the Part Navigator
  3. Reusing NX Roles in later versions
  4. Hidden Predefined “Form” Features still viable
  5. Create New Parent

Utilities Group in the Top Border Bar

When the new paradigm of the NX9 Ribbon Bar was released and thrust upon “toolbar-based” users, shoulders slumped, foreheads wrinkled, and silence was broken with words indicative of a level of joy so low that, well, there just was no joy. Now that they’ve had some time to perfect their NX OCD, they might be feeling better about it.

But if you waited to make the jump from pre-NX9 to NX9 or later, here’s a little tip that can definitely save you some clicks and put life a little closer to your reach.

In the Top Border Bar (used to be called the Selection Toolbar) there are Groups within it that can be very easily customized. There’s a whole group for Utilities set to off by default. This has some nice, commonly used commands in it.

To quickly turn the Group on, simply click on the drop-down arrow at the end of the Top Border Bar and you’ll see the Utilities Group at the bottom of the list of groups. If you hover over it, a cascade will appear to the left that includes all kinds of goodies.

Top Boarder Bar drop-down, hover over group

Now turn these options on in the Top Border Bar simply by clicking on that Utilities Group in the drop-down to turn on the check mark and then slide to the left and start turning on options.

The top border bar in NX.

Personally, I like a few of the options in the WCS Drop-down cascade like the old “Set WCS to Absolute” when you want it to go back “home.” If you’ve found it a little temperamental sometimes to get into WCS Dynamics by getting that preview to show up before double-clicking it, now you can easily turn that mode on with 2 clicks in the Top Border Bar.

WCS Dynamics in NX

Details Panel of the Part Navigator

The Details Panel of the Part Navigator can make editing parameters of features very convenient. This is especially true of editing the expressions. It comes down to merely double-clicking on a parameter in the list, typing the new number, and hitting Enter.

For example, here’s a little paddle flipper for an assembly machine that works in a wet environment. There are some drain holes on both ends so the cored-out areas don’t fill up with fluid.

Paddle Flipper

The Part Navigator lists the various features including those drain holes.

If we’re finding that those holes don’t allow the fluid to drain fast enough and it’s getting filled up, then we can increase the size of those holes. Obviously, we could double-click on a hole in the graphics area and the feature dialog would appear in which we could type in a new value. Then we’d need to choose OK or maybe hit MB2 to finish the edit.

And since there are only two Simple Hole features in the part, it’s not hard to figure out which features in the list correspond to what we see in the graphics area. But here’s the trick:

If you simply click on the Details Panel drop-down and then select one of the Hole features, all of the parameter information immediately displays in the panel.

Part Navigator in NX
Part Navigator in NX

Parameters are labelled nicely so it’s obvious which “p” number is which. Double-clicking on the diameter allows you to type the new value.

Parameter details in NX

Hit Enter and the edit is complete.

OK, maybe, if you’re counting clicks, that’s not so much faster or easier than double-clicking on the graphics area. But now you can just single click on the other hole, double-click on the expression, type the number and hit Enter and that one is edited!

Details in NX

Imagine if you had to make minor edits to dozens of features, perhaps after a design review or a first part inspection. These could all be incorporated very quickly and without the delay of dialogs displaying and choosing OK in each one. Lastly, if you press MB3 on an expression, an option to access the Expressions dialog appears to make advanced edits and references.

Editing a diameter in NX

By the way, you may have noticed that little red cone in the picture of the paddle flipper.

That is actually an injection molding gate that was defined during a mold flow analysis process. This is part of NX’s Mold Wizard product and is a very useful tool for visualizing not only the flow of material into a molded part cavity but also temperature differentials, air pockets, draft issues, and many other molding concerns that could cause problems after the mold design is complete.

For further information about this, contact your Swoosh Customer Sales Executive.

Reusing NX Roles in later versions

A question that I’ve been asked many times in class, usually while teaching a lesson on NX interface and Gateway, is if you can use a custom Role in a later version when you upgrade NX. The answer is yes and it’s very easy. Use the “Load Role” command and select the base Role “.mtx” file from the previous version folder.

Assuming you’ve already created a custom role in an earlier version of NX, the first thing you need to do is know where the actual base file for that role resides on your computer. Like most applications, personal data such as customizations, log files, history, custom tools and such, are saved in your username folder, usually inside of a folder named for that application, such as “Siemens,” and down into a couple system folders created within that application folder. For NX8, as an example, the pathname actually includes a folder named “Unigraphics Solutions” instead of “Siemens”:

C:\Users\garrett.koch\AppData\Local\Unigraphics Solutions\NX80

Within that NX80 folder you’ll see the personal, custom data and a folder called “roles”:

NX Roles Folder

Within that “roles” folder you’ll see the base files of the roles:

Base File of NX Rolls

Remember, when you create a custom Role, you define a display name which is what will appear when applying a Role. When you want to change your Role, the easiest way is simply to choose the Role tab in the Resource Bar and select the desired Role:

Role tab in the NX Resources Bar

When you create or edit a Role, you’ll see the actual base file of the Role. In this particular case in NX8, the base name is nx_role1.mtx:

Role properties in NX

Now let’s find out how you “load” that role in a later version. Because those base Role files are saved into a specific version folder, “NX80” in this case, they will not be visible in later versions on that same computer. You could go to a Windows file manager window and copy the NX8 base Role file into the equivalent folder of the desired version but that’s not recommended. It doesn’t give NX a chance to properly translate or upgrade that data.

Just to save you a bit of frustration, ignore the “Open” option you’ll see when you press MB3 on the Roles panel of the Resource Bar. It doesn’t allow you to open a base role file, only a “palette” file.

Open Base Role File

Instead, there is a command in NX that allows you to load a role into an NX session, which therefore allows it to save it into the proper folder. Up through NX9, the command was accessed through the Customize dialog which contained a tab for “Roles”. In that tab, there are “Load” and “Create” buttons:

Customize Dialogue in NX, load and create roles option

It also notifies you as to which Role was the last to be applied, whether manually or because of a custom default setting.

In NX10, the Roles controls and settings were moved from the Customize dialog to the User Interface Preferences. NX11 retained that so we’ll use that as the sample version for loading the Role.

Choose File->Preferences->User Interface and select the Roles tab. You’ll see all those same controls and settings and the Last Applied Role, in this case, “Advanced”:

Roles in User Interface Preferences in NX

When choosing the Load Role icon, you simply browse to the folder where the desired base Role file resides, “NX80” in this case, and when you select a “.mtx” file, choose OK. We select the Role file “nx_role3.mtx“ with the display name “Alex-1.” You will see the same popup that displays whenever you change Roles:

Load Role in NX

If there were any differences in the NX window layout, icons on or off, etc. that will update immediately. The status of the NX8 Toolbars will equate to Ribbon Bar Group settings in NX11. Choose OK in the User Interface Preferences dialog and it’s finished.

Be aware, however, that this doesn’t actually add a new custom Role to the list in the Roles tab of the NX11 Resource Bar. But if you go back to the User Interface Preferences, you’ll see that it not only brought in that customization data but the custom display name, “Alex-1” as well.

Last Applied Role

You simply need to save a new Role now in NX11 or whatever version you were working in.


Hidden Predefined “Form” Features still viable

Today’s CAD systems appear to all be very sketched based. The building of the first solid feature is the result of some sort of swept sketch, followed by more sweeps, whether they be extruded, revolved, or swept along some form of guide or path. However, NX contains many commands that involve “predefined shapes” which require no sketches.

When the first version of solid modeling Unigraphics was released (10.0), there were six commands that, throughout the subsequent releases, remained in some sort of grouping together. There were dialogs with text buttons, palettes of icons, and selectable items from menu drop-downs. All based on mechanical fabrication or machining operations for the most part, they included:

  • Hole
  • Boss
  • Pocket
  • Pad
  • Slot
  • Groove

Through the decades, a few more options and enhancements were added along with a new function in the group here and there. When EDS acquired all of the holdings of Unigraphics Solutions and that of SDRC’s Ideas, the Unigraphics “Hole” command was basically replaced with the Ideas “Hole” command. In more recent versions of NX, all these commands have taken a bit of a back seat in the interface and customization must take place in order for the icons to be available on the Ribbon Bar.

More than half of the students that we teach remember these commands and about half still use them. It has also become known that Creo and SolidWorks now have equivalent commands. So maybe there is some credence to this approach to adding secondary shapes to parts with predefined features.

In NX11, these commands can all be added to the Design Feature Drop-down in the Feature group of the Ribbon Bar very easily. Select the Feature Group Options drop-down arrow, follow the Design Feature Drop-down cascade over to the available icon options and just start clicking to turn on the check marks.

NX Design Feature Drop Down

The commands are now immediately available in the drop-down:

Design Feature Drop Down

But there’s one command that’s still missing: the original NX5 Hole feature. As mentioned above, it was more or less replaced by the Ideas version of the Hole command. In actuality, the “Pre-NX5 Hole” command as it is now called, was eliminated from the available Design Feature Drop-down options but not completely removed or retired. To be able to use the command, the icon must be added to the interface somewhere using the Customize dialog.

Through any of the 8 or 10 different ways to access the Customize dialog, bring it up. I prefer the method of just placing the cursor on any icon anywhere in the Ribbon bar and pressing MB3. At the bottom of the popup, choose Customize.

Customize Through Curve Mesh

 In the Search filter on the Commands tab of the dialog, just enter the characters “pre” and press Enter. (The “All Commands” category must be highlighted.)

Searching for all commands

Now you’ll see the command in the first few in the list. Simply drag it with MB1 to wherever you want, including into the Design Feature Drop-down next to the other “Form Features.”

Drag and Drop features in NX

Or you just park it next to the newer Hole command that is in the Feature group by default:

Hole Command Feature Group NX

Now you have 1-click access to the PreNX5 Hole command and 2-click access to all the other predefined features.

This article won’t get into the specific functionality and process of using these commands. But it is worth mentioning that, since the deemphasis of these commands due to the prioritization of sketch-based commands in NX, there really hasn’t been much enhancement or development done with them. This is unfortunate considering the speed and productivity they can provide.

As an example, creating a Pre-NX5 Hole on top of and concentric with the top edge of a Boss takes 7 clicks of the mouse. That creates a parametric feature that is fully associative, not only to its placement face but also to the through face. Its positional associativity to the boss is also locked in. That captures design intent just and an extruded sketched circle having all the same associativity. But the Pre-NX5 Hole can be complete in less than 10 seconds!

Create New Parent

The final item in the Top 5 list is just a quick reference to a simple command that is somewhat unobtrusive: the Create New Parent icon in the Assembly tab of the Ribbon Bar.

Create New Parent Assembly Tab NX

Simply put, this command saves you the time and effort of using 2 commands that give you essentially the same result: File->New (and choosing the Assembly template file) and then using Add Component. As the “Balloon Tooltip” displayed above conveys, the current Displayed Part will immediately become a Component in the new assembly.

This is not a process to be used in creating a Master Model scenario for drafting, manufacturing, analysis, or any of the processes that can take advantage of that approach. This is simply for the creation of a standard assembly.

There are some other concepts that should also be clarified:

  • In this scenario, the model position of the current Displayed Part will be defined as it is in that Displayed Part. So, whatever point of the model geometry is at ABS 0,0,0 will also be at ABS 0,0,0 in the resulting assembly file. Or if the model geometry is located away from ABS 0,0,0 in model space, as might be the case in the automotive, aerospace, and aeronautics industries where they use a VCS (Vehicle Coordinate System), then that model geometry (Component) will still be in the same position in the assembly file. In other words, the origin of the Component in the assembly as it’s being created is like using the “Absolute Origin” option in the Placement group of the Add Component dialog.
Placement Absolute Origin

Placement Absolute Origin

  • The “Entire Part” Reference Set of the current Displayed Part, used as the assembly file, is created and becomes the new Displayed and Work Part.
  • There will be no Assembly Constraints created. Therefore, it would be wise to immediately add a Fixed Constraint to that one Component. Also, in planning this whole approach to building the assembly structure using Create Parent, it would be wise to make sure that the current Displayed Part that you are working on is one of the most important primary parts in the assembly. A frame, baseplate, or housing part would be a good example.
  • If you are in the beginning stages of designing an assembly structure, it is not out of the question to use this Create Parent command multiple times in a row to quickly establish the multi-level structure. Or, you could even create them in a vertical structure and then start dragging subassemblies up or down the structure to establish lateral subassemblies within a single, higher level or top level assembly. That is a very fast approach compared to changing the Work Part and using Add Component.
Assembly Navigator NX

Important: get the file names exactly correct while you do this because changing names of any lowest level Components, subassemblies, or top level assembly gets cluttered and clunky. You end up dealing with fairly complicated Replace Component and Save As operations. For example, if you had made the bottom level Component the Work Part and then performed a Save As to change its name, NX is going to prompt you to save as on each level of that assembly all the way to the top. You type a new name and choose OK and the dialog appears to close but immediately pops right back up and you usually can’t see what it wants because Information Window that reports it all is hiding the Cue Line. And it won’t let you move it out of the way because the active focus is on the Save As dialog.

Save As Dialogue NX

Well, we hope this little smorgasbord of side topics has been useful enough to make you consider when the last time was that you had training. Our classes are chock full of tips and tidbits like the above that give more advanced users some insight into increasing productivity and getting the job done a little faster, a little better. We still teach all the fundamentals of CAD and those advanced topics that are only found in the more capable systems like NX but these little nuggets really give you a sense of value for the time and budget that you spend while getting training.

Thanks for hanging in!

Post by Garrett Koch

Leave a Reply

Your email address will not be published. Required fields are marked *