Rapid Dimensions Drafting NX9 3

[peterrdevries]

Working with NX9.0.0.19 in Drafting Rapid Dimension with Tolerance. Hoe easy is was to place a Tolerance, the more work it is in NX9:

- Place a Dimension -> mb3 -> Tolerance -> buttons in front of Tolerances are not there!

- Place a Dimension -> mb3 -> Tolerance -> f.e. Equal Bilateral Tolerance -> change the Tolerance ...... now the amount of mouse clicks is too much: do not move the mouse -> Edit button -> then select the green/brown rectangle -> change the Tolerance Value -> de-select the edit button ( DO NOT press middle mouse button, what all user do... -> dimensin is gone -> start all over) -> Place the dimension.
When reading press releases about less mouseclicks in Drafting, then .....

Another one is the Appended Text, a lott of NX Drafters are using the 4 Arrow Keys on the keyboard when creating appended text -> not possible anymore. Use a dialog instead.

Anyone experience with all of this? Are we doing anything wrong in creating Tolerances / Appeneded Text in NX9?

 

[cubalibre000]

It's normal no icons on the RMB like the image attached ?

Thank you...

Using NX 8 and TC9.1

 

[peterrdevries]

Cubalibre,

I thinks this is not normal. Icons should be there. Hopefully next release.

JohnRBaker,

I understand your video and the way of working. We have to get used to it, but users complain about more mouseclicks when placing a dimension with tolerance (than in previous releases), and they are right.....

Peter

 

[peterrdevries]

The behaviour as decribed above (Rapid Dimension from Centerline to Edge) = Angular Dimension.
See attached video.

Peter

 

[peterrdevries]

now with correct video, sorry

 

[carlharr]

Peter, select the endpoint of the line instead of the line, and it should work.

That one keeps catching me out, but I think its because rapid dim captures more options now, so you need to be more carfeul than before with selections.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[peterrdevries]

Carlharr,

I know i need to select the point, BUT, can you imagine how to explain this to users who are used to simply select the Centerline they were used to in previous releases? That's my point in all the issues concerning Rapid Dimension.

Peter

 

[carlharr]

Peter,

I mean then endpoint of the edge, you can still select the centreline as normal. That said, I'm still struggling most with dimensioning for a few reasons, planning to do some more work on it next week.

Carl

http://www.jcb.com

NX 7.5 with TC 8.3

 

[peterrdevries]

Carlharr,
Thanks for that tip. I was not aware of selecting the edge first.

Peter

 

[JohnRBaker]

The Tolerance pop-up icons are working juat fine in NX 9.0.1...

John R. Baker, P.E.
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[JohnRBaker]

From a post on 20 Jan 14 11:49...

As for selecting a dimension to edit while the 'Rapid Dimension' dialog is open, that does appear to have changed despite the fact that when the dialog is open the Que/Status line still says that you can 'double-click to edit'. At the moment, you need to simply double-click a dimension (with no dialogs open) to launch the 'edit' mode. However, I will open a PR since either the Que/Status line is incorrect or if it is correct, then the edit function isn't working as it should.

I just got a response to my PR. Apparently it was decided, and understandably so, that it was confusing to allow someone to BOTH create and EDIT a Dimension from the SAME dialog entry. Granted, as I had already mentioned previoulsy (see above quote), if you were to double-click a Dimension without the dialog open, you would see a dialog that looked virtually identical to the Dimension creation dialog, but you would be in the edit mode. Besides, this would also be consistent with most of the rest of NX. For example, if you were to open say the Extrude dialog, there's no option there to edit an existing Extrude feature, however, if you double-clicked an Extrude feature you'll get, as I mentioned before, a dialog which is virtually the same just dedicated to editing and not creating an Extrude feature.

That being said, they did agree that the Que/Status line was incorrect and so they will be changing it to remove any reference to using the dialog for editing an existing Dimension.

John R. Baker, P.E.
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Product Engineering Software
Siemens PLM Software Inc.
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[carlharr]

John,

On a vaguely related note, NX9 sketch origin in the create sketch dialog, I'm finding that it keeps defaulting to endpoint when I select a face, instead of inferred (which would follow the snap points).

Even if I've previously used create sketch with inferred origin, so that it's stored in the dialog memory, as soon as I click a face it returns to end point.

Are you seeing the same behaviour in your newer version?

Thanks, Carl

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

That behavior actually changed starting in NX 8.0 as part of a rather subtle enhancement with respect to both the 'Point/Origin' portion of all Modeling dialogs as well as a change in behavior when you edit any feature which used the 'Point/Origin' function when creating the feature.

As I alluded above, the NX 8.0 enhancement had two parts, the first being that in all Modeling dialogs where there is a 'Point/Origin' option you now have the option to display a list of 'Shortcuts' for the most often used 'Point' options and this is available whether the 'Snap Points' in the Selection Bar are active or not. The second part of the enhancement is actually the really subtle part and that is that when you create any sort of feature that involved selecting a point, whether it was an explicit selection or not, that method used when creating the feature is actually saved as part of what we call the 'feature method' however most people were not aware of that even though you could edit that when the edited the feature just that there was no indication as to exactly what point method was originally used when you created the feature. That all changed starting with NX 8.0. Now when you edit the feature and the dialog for that feature opens, in the past the 'Point/Origin' option always reset to 'Inferred' despite the fact that that's meaningless since 'Inferred' is NOT actually a method used, but rather just a way to indicate that you can select anything that you want to select but it gives you NO feedback as to what was used when the feature was created. Now it does. So if you create say a Block feature where you selected the 'End Point' of curve when you edit the Block it will now show that indeed you DID use an 'End Point' because the 'Point/Origin' will show an 'End Point'. We're just providing MORE feedback about how the feature was actually created. For many people this could prove to be a very useful bit of additional information.

Now exactly how did this change what you're seeing when you create a Sketch. Well in those situations where making a selection in some other part of a dialog causes the 'Point/Origin' selection to be made automatically, while in the past even though something WAS selected there was NO indication what that Point method actually was even though you could probably guess by looking at the feedback on the screen. Now when the inference has been made the dialog is updated to show you what Point/Origin method WAS used. In the case of selecting say the face of a Block to create a Sketch, in reality, and you can clearly see this, an 'End Point' of one of the face edges was selected as the Origin which is why the 'Select Origin' switched to 'End Point'. Note that if you had selected a Datum Plane it would have switched to 'Fixed' and if you had selected the end of Cylinder it would have switched to show that the 'Arc Center' method had been used. Now I will admit that this does not provide as much additional functionality when working with Sketches since editing a Sketch does not automatically use the original dialog, unlike other features where you are given the opportunity to edit the 'Origin' and thus it would be useful to know what method was used originally.

Now before you comment on the fact that in NX 7.5, since it always defaulted to 'Inferred', that when you made the 'Point/Origin' entry active that this would also make the Snap Points in the selection bar active and so now you have to make an additional selection, back to 'Inferred', before that's the case, let me remind you that you now have the option to show at least six of the most recently used point methods in the 'Shortcut Toolbar' in the 'Point/Origin' section of the dialog so that those methods are always available irrespective of what the default method was set to. You can use these six additional icons (actually five since the current one will always to shown in the Shortcuts) to change the method used if you really wanted something other than what the Sketch function had inferred by how you had selected the Sketch plane.

BTW, this same behavior change can be seen wherever a feature which uses a Vector, including providing you with the optional Shortcuts as well as the feedback when editing a feature which used a Vector as part of its 'method'.

Anyway, I hope you can see how this subtle change is actually a rather nice enhancement when you understand what's happening and how you can leverage the additional information now shown to you, both during creation and editing, although this last aspect is not as applicable to Sketches as it is to most all the other Modeling features, but hey, it's at least consistent.

John R. Baker, P.E.
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[carlharr]

Hi John,

Thank you for the detailed answer. I've tested the difference in 7.5 and 9 ref. your block examples, and I see how the origin selection method is now "remembered" in the feature, subtle but the difference is there.

I can also see how this isn't really necessary for sketches, but as you say the dialogs are consistant.

The shortcuts do make this easier, in fact with shortcuts already displayed it's the same number of clicks as 7.5 (in 7.5, expand origin and click Specify Point, in 9 expand orgin and click Inferred shortcut).

So my question that follows from this - is it possible to set the dialogs so that they always display the shortcuts. When I hit the reset button they disappear, and I'd like them to stay.

Thanks again, Carl

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

Unfortunately, the default shortcuts setting is OFF since it was felt that if we turned them all ON that the dialogs would become longer and many are already pretty long as it is. And besides, it's not just the Point shortcuts, there's also the Vector shortcuts so if you turn them on as well, and since many dialogs have BOTH, well, you get the point... And before you suggest it, it would add another level of complexity if we started to make it user controllable as to which parts of a dialog would be subject to being reset versus which parts would not. Which begs the question, why are you resetting the dialogs in the first place?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
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[carlharr]

Hi John,

I reset (mainly) because of remembered selection intent rules, which are almost always wrong the next time I use a command. Defaults for selection and all other options are normally the most useful, and are the ones that stick in my mind as "the way a command works".

It has become automatic for me to hit reset straight away, so that command behaviour is predictable and NX is faster.

Maybe I need to change my methods...

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

We intended Dialog Memory to provide users with a sort of 'adaptive' behavior where the options are retained, particularly during periods where several operations are performed in a sequence where most of the settings are not going to change from one use of the dialog to the next.

That being said, if it's more control of what the 'default' content of a dialog is that you're looking for, perhaps you should look into using the 'Favorites' feature. When a 'Favorite' is being used, the 'Reset' option only acts on the numerical entry fields and not on the options nor the structure of the dialog. For example, take the Extrude dialog; if you wanted the Default to always have the vector shortcuts displayed and the default Boolean set to 'None' with only the Settings and Preview sections collapsed, you could set-up your dialog that way and save a 'Favorite'. Then when you hit the 'Reset' it would take you back to the state that the 'Favorite' was last saved but the Start and End distances would be set back to their actual deafults of 0 and 25. And keep in mind that which Favorite was last used by a dialog will be retained by Dialog Memory. So you could literally customize all of your dialogs, in essence redefining most all of their 'default' content and options, and simply use these 'Favorite' definitions rather that what the OOTB 'Reset' defaults would have been.

Anyway, give it try as I think you'll like it. However, one comment, as you've already sort of figured out, the Sketch Task dialog is sort of a hard-case having it's own special behavior and it's true here as well as it appears to not have the same 'Reset' behavior as does other dialogs. Now this might be a simple bug and I'll check that out and if so, I'll open a PR, but when with that in mind, you should at least look at setting-up 'Favorites' for your other most often used dialogs and get them to start behaving the way you want them to.

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.

 

[carlharr]

Hi John,

I had a go with favourites, by creating a simplified extrude as per the help material, to see what it did.

Whilst it worked, I ran into some problems in that:
1. once I'd created "Simple Extrude", the original dialog had the same name as my favourite and wouldn't change
2. there's no way to delete favourites, I had to go to C:\Users\<username>\AppData\Local\Siemens\NX90\Favorites in order to delete and while I can do this, all of our users wouldn't have access to do so

So I decided to leave favourites alone for now and come back to them.

That said, I've just created a Sketch in Task favourite ("Sketch Carls") with the shortcuts shown. Seems to work ok except... I've now deleted the favourite file and the favourite won't go away - my Sketch Task now seems to be stuck on the new "Sketch Carls" even though this isn't an option in the settings any more.

Will try restarting the computer.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[carlharr]

I've now also deleted the dialog memory file and that's cleared all traces of my favourites.
For a few reasons, I will leave favourites alone for now.

Back to the original question (sketch origin in create sketch not defaulting to inferred once a face is selected)...
I do understand why the default now is inferred only until you select a face, after which it changes.
It's a shame, because you'll only want to specify a sketch origin after the face was selected. Since create sketch is a relatively important dialog, maybe this behaviour will be modified for this dialog only in future.


I don't think there's anything wrong with reset behaviour, simply that reset clears away the shortcuts (which are the simple workaround to the "problem" above). I will have to avoid re-setting create sketch!

Thanks for your help, Carl

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

The issue with the Origin option being forced by the face selection is that actually TWO actions are resulting from this single selection, identifying the plane that the sketch will lie on AND what the origin of the sketch will be is determined by the type or shape of the planar object that you selected. In essence, this is the ultimate in inferring the origin. And while it is true that this causes the 'Snap Point' options to be made inactive since we now automatically set the origin option to whatever was inferred, it does provide that additional level of feedback showing what the system ACTUALLY did when it inferred the origin method. And while it may be true that perhaps in the case of Sketches, this is not as useful since the editing scheme is different, it's ultimately a consequence of us trying to use efficient coding practices by reusing common sets of tools so it's easier to maintain the software and so that the user has a consistent experience when peforming common tasks, both of which are highly desirable, for ALL parties involved over the long haul.

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.