Basic NX11 questions 3

[fraudster]

Hello all, thanks for all the helpful contributions I see here. I am no cad expert so I have a question: Why do companies use NX, when it appears to me to be 20 years behind some other cad programs (user interface, functionality, productivity)? I have listed a few basic things I have noticed that I have not been able to resolve.

1) Eliminate distance culling.
2) Application ribbon should indicate what application is active. (Modeling, Sheet Metal, etc.)
3) Allow multiple profiles of sketch to produce sheet metal Tab.
4) Allow multiple edges to be selected in Flange command.
5) Active (or relevant) ribbon tab should be indicated, or others greyed when in command.
6) Add sketch (point) based pattern feature.
7) Make sketch constraints robust unless removed.
8) Allow sketch to be created (extracted) from face features.
9) Allow tangent lines to be displayed independent of edge lines (model view).
10) Allow assembly level fastener features.
11) Show edge lines in (model) section.
12) Allow hiding of origin to dimension lines with ordinate dimensioning.

 

[NutAce]

If you don't like it then use something else I would say

Points 6,8 and 11 are possible in NX11
And for the rest I would say, create an Enhancement Request at GTAC and become a Beta tester.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX11 / TC11

 

[Xwheelguy]

2 is done but not with anything beyond Modeling/Drafting. So what's it supposed to say when in Sheet Metal with Assemblies toggled on, "Modeling Sheet Metal Assemblies"? Seems a bit of a stretch, IMO.
5 won't happen because you can invoke commands within a command - you can measure when creating a feature, for example.
7 needs clarity or a solid example of what you mean - robust is too general.
9 can be done with Smooth Edges, both in Modeling and Drafting - check your Visualization Preferences (for Modeling) or refer to the Help docs if you don't understand how to set things correctly.
10 should be able to be done but I believe you'd have to build it yourself.

Companies use NX because it can open parts dating back to the 90's without a glorified translation - NX is an older software that hasn't had a line drawn in the sand due to a complete rewrite of the software. It also handles enormous assemblies much better than some - plus there is Teamcenter which is used by all of the Big Three automotive makers in North America and 2 of the 3 use NX as their base CAD software.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[fraudster]

Thanks for the great responses. We do handle enormous assemblies at my workplace.

With the response help I have been able to resolve 8 (project curve) and 9 (smooth edges). 7 looks like a mistake by me. The others I am looking at. Cheers

James C
NX11/TC11

 

[deedub777]

1) Eliminate distance culling.
What does this mean?
2) Application ribbon should indicate what application is active. (Modeling, Sheet Metal, etc.)
Current application shown at the top of the NX window
3) Allow multiple profiles of sketch to produce sheet metal Tab.
Introduced in NX12
4) Allow multiple edges to be selected in Flange command.
Introduced in NX12
5) Active (or relevant) ribbon tab should be indicated, or others greyed when in command.
Wouldn't this cause a bit of a light show with things greying out and back again all the time?
8) Allow sketch to be created (extracted) from face features.
Start a sketch, Project Curve (with face edges selection intent)
11) Show edge lines in (model) section.
12) Allow hiding of origin to dimension lines with ordinate dimensioning.

 

[Toost]

All systems has their "rules", limitations and methods.
NX is often "limitless" compared to other systems, -You do not need to do "a-and-b-and-c" in NX as you do in system X.
But, NX also has plenty things we would like to get enhanced.
Some responses :

1) Eliminate distance culling.
Please explain this question.
- The need to press "Fit View" ?

2) Application ribbon should indicate what application is active. (Modeling, Sheet Metal, etc.)
The NX Window border does , in text, print the active application. Do we need more than that ?

3) Allow multiple profiles of sketch to produce sheet metal Tab.
Do i understand this correct: , - separate islands or non-trimmed geometry or multiple tabs created by 1 feature ?
separate islands or multiple bodies in one feature is not supported in the Sheet metal ( -It is in general Modeling.)
non trimmed geometry, is a "selection intent" thing, a matter of selecting the correct selection rule.
( try the "region boundary curves" or toggle the Stop at intersection whilst using the "connected curves" )

4) Allow multiple edges to be selected in Flange command.
Yes, Why not. -submit an enhancement request to GTAC.

5) Active (or relevant) ribbon tab should be indicated, or others greyed when in command.
Why ?

6) Add sketch (point) based pattern feature.
Has been there since several versions back. It is the option named "general" in the pattern dialog.

7) Make sketch constraints robust unless removed.
What systems are we comparing here ?
Several other cad systems are using the same constraint engine as NX.
pls explain more.

8) Allow sketch to be created (extracted) from face features.
This is often not needed in NX, you can use the edges or faces without the extra sketch thing. ( try extrude an edge or a face for example .)
IN the sketcher you can extract necessary edges. You cannot create a sketch based of extracts.

9) Allow tangent lines to be displayed independent of edge lines (model view).
pls explain more.

10) Allow assembly level fastener features.
In NX this has been possible since early nineties, but you must first "allow" it by either creating a Promotion or a wave linked body.
since a few relases back you can also do this on the fly by toggling the "create interpart link" button when doing that feature.
( There are companies who have rules against hard geometric links between their files. - This option can be disabled in NX)

11) Show edge lines in (model) section.
This is an option you ( must... ) toggle on.
edit the section (in the top of the assembly navigator) - section curve settings - show section curves preview.
- I do not know why this isn't default on.

12) Allow hiding of origin to dimension lines with ordinate dimensionin
I do not know if this is possible or not.


Regards,
Tomas

Edit: - I see i was a bit slow pressing "submit" on this.

 

[JohnRBaker]

Number 5 would create a situation where you would have to first COMPLETELY LEAVE the current function before you could select another one. This would, in effect, add an EXTRA keystroke every time a user wanted to abandon what he was doing so as to launch a totally different function/operation.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[fraudster]

Thanks for the great responses. Most of my issues have been answered or due to my inexperience.

By distance culling, I meant that in an assy in a large area with small items, some appear to disappear depending on zoom level.

Cheers,
James C

 

[looslib]

At least NX does not revert back to the PFK icon box when it hits an older function.
The software I use now still has old menu boxes pop up at certain functions even though we as users were told 15 years ago that the menus were going away. Two name changes and software cleanup efforts and they still pop up!

The best thing about NX is the ability to do the same function in multiple ways.
The most frustrating thing with NX is the ability to do the same function in multiple ways.

At lest with NX, you can install an initial release of a version and not worry if it will crash when creating a simple cube. I had a pre-release of the other software I use do exactly that. The pre-release was issued to hundreds of customers to test te revised user interface.

I have used CAD since 1978. Applicon 880, Computervision CADDS4, CATIA V5, SolidWorks, Pro/Engineer (from 2000i2 to Wildfire to Creo), Medusa, Unigraphics (from UGII v3.2 through NX1 and then NX4 and NX6) and some versions of AutoCAD since R14 (I have 2013 loaded).


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

Ben Loosli

 

[JohnRBaker]

As I always said, with NX(UG) there's always good news and bad news:

The good news is that there are 10 ways to do everything.

The bad news is that nine of them are perfectly valid.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[Toost]

The distance culling is a performance setting to better handle large assemblies.
Imagine looking at say a ship, and you have to wait for the tiny screws in the xyz equipment to regenerate the graphics. ( so small they would be more or less invisible to the eye, but still require the CPU to process)
You can set that under Preferences - Visualization Performance - Large model - Model size : Set that to "Small" and it will not do the culling, "Large" and it will do the culling.

The "Moving frames" will simplify the graphics when rotate/zoom/pan
You can disable this too if you find your graphics runs ok.


Regards,
Tomas

 

[Toost]

Yes, this is the NX i know:
Looslib:
"The best thing about NX is the ability to do the same function in multiple ways.
The most frustrating thing with NX is the ability to do the same function in multiple ways."


Tomas