Setting dimension preferences.

[tomstickland]

One thing that really annoys me about nx6 is that for every radius and diameter dimension I have to manually edit the style to make the text horizontal and manually placed.

I've look at the preferences, but they seem to apply to all dimensions.

Is there any way to set the preferences so that radius and diameter dimensions can have horizontal text, and all other dimensions have aligned text?

There are countless other things that I think are highly illogical, overly time consuming or badly thought out in nx/unigraphics, but I'll go through them another time.

 

[ewh]

Take some time to study the options available in File -> Utilities -> Customer Defaults
This is the first thing I check when using a new version.
If you don't have the necessary permissions to edit and save to the Site Default Level, have someone who does make the changes for you.
There is much to go through, but I am confident that you will find what you are looking for if you try hard enough.


"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JohnRBaker]

Our drafting preferences are based on the various International Drafting standards which we support, therefore unless there's a 'standard' which allows ISO-like linear dimensions and ASME-like Radial/Diametral dimensions, we don't support it. Now if this is allowed in one of the standard, please let us know and we'll investigate, but as far as I know what we comply with the standards which we claim to support.

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.

 

[tomstickland]

I'm just looking at BS 308: part 2: 1985
7.1.4 Dimensioning circles
It shows a small diameter circle with a diameter dimension on it. The dimension text is on a leader, with horizontal text.


Is it possible to configure NX so that hole notes obtain all of the hole information and display it?
For example, with a cbore hole, can it automatically generate a heard with the cbore information in it?

Can a threaded hole be dimensioned so that the thread pitch is automatically added to the hole note?

 

[tomstickland]

BS 8888
see page 36 of this:

http://www.tech.plymouth.ac.uk/dmme/dsgn131/DSGN131_Course_Notes.pdf

I want a dimension like the left hand example in 2.5.3.3

 

[looslib]

That is a hole dimension in NX4.


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

Ben Loosli

 

[JohnRBaker]

That's a nice document covering the basics of drafting but I didn't see any mention or claim that what we saw therein complied with any one specific standard. In fact, I saw examples which exhibited characteristics of both ISO and ASME style dimensions. I suspect the the purpose of this 'course' was a broad review of drafting practices, but nothing specific in the way standards are used.

That being said, you already have the ability to make your drawings appear as you want them to (manually edit the radius/diameter dims), so there is NO lack of 'ability' to perform, but rather only one of 'ease' of performing. Therefore, if you wish to contact GTAC and have them open an ER, asking that this be made easier to do by adding a separate formating option for radial/diameter dimensions than from linear dimensions, that seems like a reasonable request. Of course, the out-of-the-box defaults won't change, but you could have more 'flexibility' in defining your own, albeit, non-standard 'standard' for your usage (which of course you can do now, except that we don't provide the level of 'granularity' that's needed in this particular situation).

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.

 

[hudson888]

If anything many of the standards do support a number of options for arrow an leader techniques that are equally valid. So working within that scope of possibilities one bugbear that causes extra keystokes almost constantly is that the automatic dimension arrow and placement type defaults to the least helpful option in my view for radius and hole dimensions. I'd like to see the arrow always placed on the same side as the text and the length of the leader free to vary. At the moment either arrows in or arrows out will free the leader length to vary so the text may be moved out of the way or aligned with other text, but you still need to force the arrows to change sides (according to Murphy's Law), more often than not. To the extent that there may be preferences within standards I think something like that may have been a more or less valid aspect of what tomstickland was getting at.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[tomstickland]

so there is NO lack of 'ability' to perform, but rather only one of 'ease' of performing. Therefore, if you wish to contact GTAC and have them open an ER, asking that this be made easier to do by adding a separate formating option for radial/diameter dimensions than from linear dimensions, that seems like a reasonable request.

Yes, I agree with you. I can do what I want, but it's not as quick or easy as I believe it should be.

As a user, anything that involves multiple clicks to do something that you 'believe' is a regular and common task creates a feeling of annoyance and frustration. This assumes that what you thin is regular and common really is.

What is GTAC and ER?

In Mechancial Desktop (Autocad 3D modelling, now replaced by Inventor) you could set dimension preferences overrides for every type of dimension if you wanted to.

I would say that the latest drafting package in NX is pretty good with respect to aligning, moving and snapping.
But every time I do a drawing I end having to manually change the preferences on various holes/small diameters.


Is there any way to make hole notes pick up the data for the hole? In the past I have added parameter links through to the model, and that worked alright, but I'm surprised that there's no set of templates that will automatically add the thread pitch for example.

 

[JohnRBaker]

Is there any way to make hole notes pick up the data for the hole?

Yes there is. Once you have you Drawing views placed, go to...

Insert -> Feature Parameters...

...and 'navigator' like dialog will come up showing the structure of your drawing and you should see a node for your part and under it an item labeled 'FEATURES'. Expand that item and you will see all of the features which have parameters which can be inherited automatically onto the drawing. These generally include any Sketches and Holes that are in you part model. You can select as many as you wish to apply at once and then when you get to the next step is asks which drawing view that you wish to place the dimensions in. Again, you can select as many views as you wish, including Isometric views, and finally hit OK and the 'Feature' dimensions will have been added to your drawing sheet.

Note that this works in both Master Model and non-Master Model mode.

Anyway, give it a try and see if this is what you were looking for.

BTW, if you set up your Drawing Templates correctly, you can make this happen automatically as you create you Drawings.

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]

What is GTAC and ER?

GTAC is our Global Technical Access Center. If you're in the US or Canada you can contact them direct at our 800 number:

1-800-955-0000

Or you can use the regular number:

1-714-952-5444

If you're not located in the US or Canada you should contact either you local Siemens PLM office or if you purchased NX from a distributor, start there.

Or you can try using our on-line services, which you can access while inside of NX by going to...

Help -> Online Technical Support ->

...where you will find a number of options which will give you many different ways of contacting GTAC or leveraging their services and tools, including opening an ER.

And speaking of ER's, that stands for Enhancement Request, which should be self-explanatory.

Sorry I missed this on my last reply.





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.

 

[tomstickland]

OK, thanks, for the info. I'll take a look at that.

 

[tomstickland]

That's a nice document covering the basics of drafting

BS 8888 clearly shows diameter dimensions with horizontal leaders as an option.

 

[tomstickland]

Yes there is. Once you have you Drawing views placed, go to...

Insert -> Feature Parameters...

I've tried this on some tapped holes, but sadly it only brings up "M4.1" and "dia 3.4" for an M4 x 0.7 tapped hole.

What I imagined was:
have a dimension called "hole note"
click on a hole
have an option for a range of templates
eg: M[nominal diameter] x [pitch] x * [thread length] depth full thread

or
M[nominal diameter] x [pitch] THRU

click on the type wanted
place the leader


At the moment I have to:
place a diameter dimension
edit the style to make it horizontal and manually placed
edit the tolerance to 0 precisions
change the diameter symbol to user defined, M

That then puts a dimension saying M4 for example.
I then manually edit the text to add the pitch
and any depth notes

 

[JohnRBaker]

If you use the new Threaded Hole Feature you will find that there are several string Expressions created for each feature which includes specification info that can be tied to notes.

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.

 

[JonSelby]

Reference Husdon888's quote ... "I'd like to see the arrow always placed on the same side as the text and the length of the leader free to vary.

Would it make sense for radii to automatically snap to the non-material side of the part. ie outside of the model???

(ps how do you quote on here!?!?)

 

[JohnRBaker]

For a complete guide yo the TGML (Tecumseh Group Markup Language) please go to:

http://www.tipmaster.com/includes/tgmlinfo.cfm?

There you will find all the various formatting information.

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.

 

[tomstickland]

If you use the new Threaded Hole Feature you will find that there are several string Expressions created for each feature which includes specification info that can be tied to notes.

OK, I'll look into that. It should be simple right?

 

[tomstickland]

(ps how do you quote on here!?!?)

You type
[ q u o t e] blah blah blah help [ / q u o t e]

 

[tomstickland]

If you use the new Threaded Hole Feature you will find that there are several string Expressions created for each feature which includes specification info that can be tied to notes.

Are you suggesting that I use the text editor, click on "Relationships", click on "Expression" icon, and then pick the relevant parameter from the list?