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pamccrac (Mechanical) (OP)
22 Jul 09 16:43
when launching the Transform function, it seems that Scale is the default type.  How can i change it to display all transformation types at launch i.e. translate, rotate about a point, rotate about a line, etc...?
I am finding that i must select through the scale options until the option allows me to change the transformation type when all i want is Translate function.

confusing, isn't it...

PMc
CNC Programmer

Helpful Member!  JohnRBaker (Mechanical)
22 Jul 09 16:51
If ALL you "want is Translate function", then may I suggest that you use...

Edit -> Move Object...

...instead.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

pamccrac (Mechanical) (OP)
22 Jul 09 16:56
thanks for the suggestion, does that offer Rotate about a Point, Rotate about a Line, or Repostion?
I will take a look at Move Object, but I really miss the Translation function dialog from NX3...

PMc
CNC Programmer

JohnRBaker (Mechanical)
22 Jul 09 18:19
May I suggest then that you open the Move Object dialog and press the F1 key as this will open a help page which will show you the various 'transform' options which are supported.

As for the OLD, OUTDATED, NON-ASSOCIATIVE, NX 3 style Transform, it is just that, OLD OUTDATED and NON-ASSOCIATIVE, and for the most part has been replaced by Move Object and a few other more modern functions, some of which have been part of NX for some time now.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

cowski (Mechanical)
23 Jul 09 9:41
Jump in to the new dialog and make yourself at home. You may dislike it at first but you will quickly realize that RESISTANCE IS FUTILE. Seriously though, take a good look at the 'dynamic' option as it is very versatile.

I'm a bit puzzled by the associative 'move' option, though (an associative 'copy' is understandable, but 'move'?). So, to the users of associative 'moves': what good use have you put this to? does it make it easier to model? easier to maintain your model? does it make your model more robust? In what situation is it necessary or desirable? What problem has it solved for you? In short, why is it a good thing?
JohnRBaker (Mechanical)
23 Jul 09 10:48
OK, for example, if you 'moved' an object by rotating about an axis and you made it 'Associative', the angle entered for the move would be stored as an Expression meaning that you could now control the rotation of that object by editing that expression.  Or if you specified a Distance along an axis, that value would also be saved as an expression.  And when we release NX 7.0 later this year, if you use the Delta Offset method then the values fro X,Y,Z offset will also be stored as expressions.

The point I'm making is that if your designs would benefit from being able to explicitly MOVE models, or parts of models (not components in an Assembly, but parts of an actual design model), this may be the tool you'll want to consider using.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

potrero (Mechanical)
23 Jul 09 12:03
One interesting use of Associative Move features is to control the location of a dumb solid in a design master.  

Let's say that you have a standard, commercial-off-the-shelf item (like a motor, for example), which defines the location of several other items in an assembly.  You could obtain a solid model of the motor from the manufacturer, import or un-associative WAVE link the body into your design master part, and then use Associative Move features to place the motor with respect to datums etc in your design master part.  Then you could use features on the dumb solid (such as mounting hole locations, shaft axes, etc) to control and define other datums etc in your design master, and in derived parts and assemblies down the road.

This might be an unorthodox approach to design masters and WAVE modeling, but it can be pretty useful sometimes.
pamccrac (Mechanical) (OP)
23 Jul 09 13:50
this is all good stuff.  however, please consider the CAM user that just wants some "quick" NC geometry.  The old style was very useful and in a competitive market, speed is everything.  that's where change seems to affect me, it's slow at the beginning.  the "enhancements" are great but usually need some time to get the "burned in" methods out and the new brain washed in.  With that thought and reverting back to the Transformation Types question, why is Scale the default and is it changeable in code?  I would really like and expect it to default to transform, but that's just me.

PMc
CNC Programmer

cowski (Mechanical)
23 Jul 09 14:21
What would you like it to default to? No doubt you have noticed that transform and rotate are no longer on that menu (there is probably some obscure method to turn them back on, but I wouldn't recommend it). If you want quick and dirty translations and rotations, I recommend you start using the 'dynamic' option of the 'move object' command.
Xwheelguy (Automotive)
23 Jul 09 14:22
Transform NO LONGER exists on the old Transform menu.  It has been REPLACED with Move Object.  There isn't any defaults controlling this and you can't make it appear by changing a default setting.  The only things available on the Transform dialog are those buttons that appear when you select the Transform command.  The rest have been moved to the newer Move Object command.

While I do sympathize with you in regards to getting used to something new, I don't think you're going to get very far with your preference for the old Transform command instead of Move Object.  Please do not think of my response here as being critical, because that's not my intent.  Basically, Siemens changed the Transform dialog at the users' request and now we have Move Object in its place.  Siemens usually doesn't backtrack to old methods unless the new methods are really poor and not really helpful as a whole.

Tim Flater
Senior Designer
Enkei America, Inc.
www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

pamccrac (Mechanical) (OP)
23 Jul 09 14:24
I have found that if i keep hitting enter i finally get to the "old nx3" dialog.  it's just a pain to get to.  that's why i'd like it to default to "translate" (i mistyped in previous post and put transform... duh)

PMc
CNC Programmer

pamccrac (Mechanical) (OP)
23 Jul 09 14:28
try it and see if you can get to the old dialog as well.  I stumbled across it and that's what i've been using for the past week now.

I'm still getting familiar with the enhancements of NX6 but my work load is backing up tremendously...  I do appreciate the help from forums like these and this, to me, is the best forum for NX.  smile

PMc
CNC Programmer

JohnRBaker (Mechanical)
23 Jul 09 15:04
OK, I finally found what you happened to discover, I assume by accident.  Whatever the case, this was never intended to work that way and is an artifact leftover from something which we would have liked to obsolete altogether.  But as such, it will NOT be 'fixed'.  Technically I was seriously considering opening a PR asking that this 'back-door' to the obsolete behavior be removed, but since we have more important fish to fry, I'm going to leave this alone and so you can continue to use it in whatever manner if wish, but I don't think it's in anyones interest to waste resources on this sort of fix, which while it may not be what we intended, it's doing no harm and so lets just leave it alone, period!

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

wmalan (Aerospace)
23 Jul 09 15:14
To all about this whole Translate vs Move. In my world Contol-t is simple. Control+shift+m is ridiculous. That is what I miss the most about the old translate. I too am an NC programmer.

--
Bill
Helpful Member!  pamccrac (Mechanical) (OP)
23 Jul 09 15:17
ah!  see, if you just hit enter enough, you'll get what you want...  lol.   
well thanks for your reconsideration of not removing this, i would definately be scratching my head then.  and maybe this will be of some help to another poor soul like myself who struggles with change smile.

PMc
CNC Programmer

JohnRBaker (Mechanical)
23 Jul 09 15:26
Under Customize... Keyboard... it takes about two minutes to change 'Ctrl+t' so that it brings up 'Move Object', instead of 'Transform'.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

MarcNeves (Mechanical)
25 Aug 09 7:29

what is missing is a simple TRANSLATE DELTA, without having to specify points and delta coordinates on the WCS.
JohnRBaker (Mechanical)
25 Aug 09 10:48
Delta XYZ was added as a 'Motion' option to the Move Object function in NX 6.0.2.8.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

wmalan (Aerospace)
26 Aug 09 15:17
"Under Customize... Keyboard... it takes about two minutes to change 'Ctrl+t' so that it brings up 'Move Object', instead of 'Transform'."

John, forgot to thank you for that. Works like a charm! Took me about 10 mins because I'd not changed keyboard shortcuts in several years. Btw, I think it should be under Preferences but... that's an Oprah for another day.<g>

--
Bill
design0058 (Mechanical)
2 Sep 09 12:57
Under the old transformations there is translate delta.  Using this function you could incrementally move an object the amount that was keyed in by hitting the move button again and again.  With the new move object and using Delta XYZ, I haven't been able to find how to replicate this.  As far as I can tell, after you move the object you have to select it again to continue moving it incrementally.  Can anyone help with this?
solution58 (Computer)
2 Sep 09 13:53
design0058

Using the keyboard hit (Ctrl t), pick your object,on the menu hit OK,pick mirror through line or plane, pick your choice in the model,next menu that comes up is the old transform menu and you are good to go, it is fast and as you know you just hit return and move as you always did in the past, not all of us care about about associativity, we care about speed and get the tool built, there are certainly some nice features in NX6 when it works without internal errors which as we were told would be fixed in NX7.

Hans
JohnRBaker (Mechanical)
2 Sep 09 14:01
That behavior, being able to apply some sort of incrementally 'additive' operations by hitting 'Apply' multiple times is generally not supported as part of the new style User Interface, however, for on screen GWIF's (the little text entry fields which pop-up on the screen) you can do something which is very close.

Now for Move Object, select your body, then using the Motion type 'Dynamic' you will see the 3 directional/3 rotational handles come up.  Select the desired one and enter your incremental value and press the 'Enter' key on your keyboard.  Now if you continue to press 'Enter' it will continue to incrementally move the body.  You can also immediately, without having to go back the dialog, select one of the other 5 handles, enter an incremental value and repeat this process of pressing the 'Enter' key until you have the final desired location/orientation.  Granted, this only allows you to enter one value at a time, but it does provide the ability to use this for both Translations and Rotations, whereas Delta is Translate only.

Anyway, give that a try and see if that will meet your needs.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

design0058 (Mechanical)
2 Sep 09 16:59
Thanks John, I'll give it a try.  Hey Hans, I agree with you 100% "not all of us care about about associativity, we care about speed and get the tool built".  I get frustrated with new releases.  Take away a few button pushes here and add a few mouse click there.  The new features are nice and needed in today's world but why does it have to take longer to get to the destination if you know what I mean.  I've been using UG since version 4 or 6 and I still think I could design simple components faster in UG version 9 than NX version 6.  Bring back the button pushes!!!!  Does anybody remember when you could hit numbers 1, 2, 3 and ? (I don't remember the last number because it has been so long) and get a horizontal line?  Try and do it that fast now.  
JohnRBaker (Mechanical)
2 Sep 09 17:39
The last number was 14.

And this what a Unigraphics 'workstation' looked like back when I stared using UG:



And if you would like to get the full story about the PFK (AKA 'the original UG user interface'), go to:

http://plmworld.org/museum/hall/History_of_the_PFK.htm

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

JohnRBaker (Mechanical)
2 Sep 09 18:31
Speaking of 'User Interfaces', I have a query;

When you are working with Drafting Symbols, the ones (usually a circle with an inscribed letter/number) which are linked to the items in a Parts List or some referenced note, when you refer to them, do you think them as an 'ID Symbol' or 'Identification Symbol'?  In other words, do we need to spell out the word 'Identification' or not?  This would be both in terms of what you would see in the user documentation as well the User Interface, such as in Dialogs, Icon names and in Tool Tips.

Now I would like to hear from users who are also using NX with non-English dialogs as well as people whose first language may not be English yet are using NX with English dialogs, what are your views on this same topic?  Is spelling out the word 'Identification' better than using the abbreviation
'ID'?
 

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

MickyV007 (Mechanical)
3 Sep 09 3:19
John,

as a Dutch speaking NX user i don't think spelling out the ID abbreviation would be usefull.  People are so familiar with the english language nowdays(school, tv, movies, music). It would be like spelling out CAD/CAM all the time, the abbreviations are common good if you work in this sector, plus it speeds up reading/speaking. So the same for the abbreviation ID.

Hope it helped a little.

Best regards,

Michäël.

NX4.0.4.2 MP10 / TCE 9.1.3.8_build_0711 / NX6.0.2.8

Belgium

solution58 (Computer)
3 Sep 09 13:56
Hi John,

"ID" symbol is perfect, the menu icon shows exactly it's intended use for a BOM or you can use it to ID anything else.

Design0058,

I go back to V-7, that old PFK was very fast, especially after one memorized the pattern, type in your commands fast enough and you could sit back and watch your model being manipulated,
time is everything in our business today, a project that had a lead time of 12 weeks twenty years ago is now expected in four and must pass FAI in most cases.

Hans
JohnRBaker (Mechanical)
3 Sep 09 14:08
We referred to those memorized PFK sequences as 'Muscle Macros'.  Of course, things could get really exciting when we moved commands around from one release to the next.  I can recall when we almost switched Delete and Blank until someone pointed out that right up to and including when stuff actually started to disappear off the screen, that the menu prompts in the Message Monitor that the user would see and be responding to were almost identical for BOTH Blank AND Delete, and that it was not until he tried to Unblank something that he would have noticed that he had deleted something instead, and remember, this was before we had Undo winky smile

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

design0058 (Mechanical)
3 Sep 09 17:05
John,
Ok, I realize those old button pushes are never going to come back but there is one thing that maybe you could help me with.  Is there anyway to assign the F9 through F12 keys to OK, Apply, Back and Cancel as they once used to be?  I've tried to use the Customize Keyboard but I can't find them there.
JohnRBaker (Mechanical)
3 Sep 09 19:59
Oh, this is going to be so easy.

Out-of-the-box, the F9, F10, F11 and F12 keys are currently unassigned so all you have to do is go into the Customize dialog, select the 'Keyboard' option, scroll about 20% down the 'Categories:' list and select the item titled 'View Popup' (the top item, not one of secondary ones) and now over in the 'Commands' column you'll find those elusive OK, Apply, Back, Cancel options.  Now all you have to do, to program the F9 key for example, is to select the 'OK' item in the Commands Column, change the focus to the 'Press new shortcut key' entry and press F9 and then press the 'Assign' button below it.  Now repeat for Apply, Back and Cancel.  Then Close the Keyboard and the Customize dialogs, and so that they don't get lost, save your Role and you should be good to go.

I said it was going to be easy winky smile

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

Helpful Member!  cyberpete (Military)
16 Sep 09 23:08

I am going to drop a bomb on this thread.

turn on / some of the legacy transformation options are not available in NX6.

UGII_ENABLE_TRANSFORM_LEGACY_OPTIONS = 1

Right click My computer - properties - advance - Envirorment variables - New -
Variable  UGII_ENABLE_TRANSFORM_LEGACY_OPTIONS
Value     1


Works great.

Don't rely on it, like John said the new fuctions in Move are better, just take some getting use to.  
JohnRBaker (Mechanical)
17 Sep 09 1:43
And some day we may just decide to disable some of these 'turn on a legacy function' environment variables just to a) see who's still using them and b) as a sort of 'warning shot' across the bow winky smile

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

pamccrac (Mechanical) (OP)
17 Sep 09 8:29
Thanks cyberpete.  Even though my collegues and I were getting more comfortable with the Move Object function, this makes for a nice transition.  Many Thanks!  smile

John, your point made is understood as well.  Thanks to all!

PMc
CNC Programmer

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