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tomstickland (Mechanical) (OP)
24 Feb 10 5:05
I've been looking at sketches on drafting views.
It's rather unclear as to what this offers over and above expanding a view.

According to the help:

Quote:

Use the Sketcher while in Drafting to create sketch curves on drawing views without expanding the view. The sketch curves can be associatively constrained to geometry in the view. The software creates the sketches as view-dependent geometry in the selected view.

When sketching on a drawing sheet, you cannot create constraints between sketch curves and member-view geometry. However, if you turn off the Preferences→Sketch→Sketch Style→SettingsCreate Inferred Constraints option, member-view geometry can be non-associatively referenced to infer positions and orientations of sketch geometry.

For me, the first problem is that the help files say that to add the sketch I should use the "sketch" icon on the "curve" toolbar. I've had a look at the curve toolbar and all of the icons that can be enabled on it and there is no sketch icon.

So, instead I looked in the insert menu and there's a "insert sketch on sheet". This does not activate the sketcher in a manner that I've ever seen before and no "close sketch" chequered flag appears anywhere.
A right click on a view gives an "active sketch view" command.

At this point I decided to use the command finder utility. On asking it where various sketch icons were it seemed to add to the insert menu an option above "insert sketch on sheet" called simply "sketch". Using this also follows no recognisable sketch routine.

I do get a load of sketching tools including constraints, but no sketch dimensioning icons and no "close sketch" icon.

So it appears that I am not actually starting the sketcher.


I am wondering whether the help files I have are out of step with the version of nx I am using.
 
cowski (Mechanical)
24 Feb 10 9:13
The sketcher works a bit differently in drafting (as you have noticed). I hope you like it because I believe it is a preview of things to come for modeling.
Helpful Member!(2)  tomstickland (Mechanical) (OP)
24 Feb 10 9:18
My conclusion after this morning is that sketch in drafting offers nothing of any real use.
It has the feel of something that was tacked on for some reason or another.
If you could add dimensions and constraints relative to the view geometry then it would be really useful.

As it is, I see no reason why anyone would ever bother using it at the moment.
JohnRBaker (Mechanical)
24 Feb 10 15:28
Please, when asking a question about a specific function or feature, tell us the version of NX that you are running.  THANK YOU!!!!

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.
 

jerry1423 (Mechanical)
24 Feb 10 15:34
I feel that is was tacked on there because that is what other CAD software programs do, such as SolidWorks. I really don't like it either - a bit of a waste of programmers time.
tomstickland (Mechanical) (OP)
24 Feb 10 16:50
I'm at home now. It's NX6. I'll check exactly which version when I'm at work tomorrow.
JohnRBaker (Mechanical)
24 Feb 10 19:07
If you don't want to Sketch in a Drawing, FINE, just use the normal tools found on the 'Lines and Arcs' toolbar instead.

Besides, I suspect that you're not even doing anything close to the type of work which we designed 'Sketching in a Drawing' to be used for anyway.

As for whether it was a "waste" of programmer's time or not, we'll let the people who actually DO know how to use it for what it was intended to be used for decide that one, OK 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.
 

LMTDCS (Mechanical)
24 Feb 10 21:56
We for one use this funtionality all the time. One area we find it very useful is adding mfg data to our parts. An example would be adding pin geometey to the drawing for the toolmakers to grind angled surfaced into position. An other example is a punch defined in 3d space. We add 2d geometery to represent the punch block that will go into the wire edm department.
John can you comment on the new drafting module in nx 7.5 yet??? As an old Ideas user it sounds as there will be alot of similar features.

L&M Tool, Inc.
JohnRBaker (Mechanical)
25 Feb 10 2:24
Yes, there is a new Drafting module, which is currently being called DraftingPlus (that may change before NX 7.5 is actually delivered), that will introduced with NX 7.5.  There will be more information available about this when we actually start the NX 7.5 launch during the 2nd quarter of this year.

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!  phillpd (Mechanical)
25 Feb 10 2:29
John, I've not really played around with this too much yet, but you state...

"Besides, I suspect that you're not even doing anything close to the type of work which we designed 'Sketching in a Drawing' to be used for anyway."

Could you give some examples ?
 

Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a Siemens PLM Solutions Partner

JohnRBaker (Mechanical)
25 Feb 10 2:57
Are you doing 2D Design and Drafting?  That is, creating Drawings which consist of ONLY 2D curves and annotation and nothing else.

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.
 

phillpd (Mechanical)
25 Feb 10 3:08
Sometimes, yes. Is that its intended audience ?

Is it also to be considered a replacment for adding geometry in an expanded view ?

Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a Siemens PLM Solutions Partner

JohnRBaker (Mechanical)
25 Feb 10 3:24
Yes, that's one of the primary market segments, but not necessarily exclusively, but close.

And NO, it's not a replacement since you can still do that using the Lines and Arcs toolbar.

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 (Mechanical) (OP)
25 Feb 10 7:27

Quote:

As for whether it was a "waste" of programmer's time or not, we'll let the people who actually DO know how to use it for what it was intended to be used for decide that one, OK

Can you please tell me what it is intended for?

I'd love to use it to add detail to drawing views and associate those to the existing geometry. This would be very useful and would be better than expanding views.

At the moment all it lets me do it put in curves and put constraints on them. I can't add sketch dimensions. I can't put constraints relative to the geometry of the view. Hence it's not much use.

I'm using NX 6.0.4.3
Do the later versions offer any more than what I have?
phillpd (Mechanical)
25 Feb 10 8:05
If you're using 'master model' then you'll have to toggle on Associative Extracted Edges from View Style to allow geometric constraints to underlying geometry.

Just create regular dimensions and you'll see that they also have an expression associated to them.

Specialty Engineered Automation (SEA)
http://www.sea4ug.com
a Siemens PLM Solutions Partner

tomstickland (Mechanical) (OP)
25 Feb 10 14:34
That sounds a lot more promising. I'll give that a go.
tomstickland (Mechanical) (OP)
1 Mar 10 11:14
I've just tried adding a dimension linking a curve to the edge of the part and I get a message saying:
"Some of the selected objects or snap options are not allowed for driving dimensions."

I couldn't find a "Associative Extracted Edges" option anywhere in the view style.
tomstickland (Mechanical) (OP)
1 Mar 10 11:15
Update: It will allow me to dimension of holes in the view. So I just need to find out how to attach dimensions to the edge of the part in the view.
tomstickland (Mechanical) (OP)
1 Mar 10 11:16
I meant "off holes".
tomstickland (Mechanical) (OP)
1 Mar 10 11:22
Update 2:
I've got it working.

In view style select "General" tab and then select
"Extracted edges" and from the pull-down list select "associative".
cowski (Mechanical)
1 Mar 10 11:30

Quote:

I couldn't find a "Associative Extracted Edges" option anywhere in the view style.
On the view style "General" tab, you will find the option right below the "Scale" option. I was looking for a 'radio button' option to choose on or off, but it is a drop down 'choose list' type of option.
tomstickland (Mechanical) (OP)
1 Mar 10 11:42
Here's my full method.

This feature allows details to be drawn on the view and the geometry constrained to the drawing view.
In most cases this is superior to the old "expand member view" method, since the geometry can be properly linked to the view and will update if the view changes.

It's taken a while to work this out, since there are many confusing details.

-Select a view
-In order to pick up lines in the view it is necessary to edit the style of the view and in the "general" tab select "associative" from the drop down list for "extracted edges". If this is not done then
the dimensions will not attach to the part and a message saying "Some of the selected objects or snap options are not allowed for driving dimensions." will occur when dimensions are placed.

-Right click, "make active sketch view". (This is not the same as doing insert-sketch or insert-sketch on sheet). In the part navigaor the view should show as "(active)".
-Make sure that the "sketch tools" toolbar is used, not the "curve" toolbar.
-Draw the sketch.
-Apply constraints as per model sketches.
-Add dimensions using the drafting dimension toolbar. These should appear like parametric dimensions, ie: allow user to set the values which then drive the sketch.
-There is a toolbar called "sketcher" that  has only the tools "delay evaluation", "evaluate sketch", "display object colour" and "text below icon".
The sketch will auto-solve every time it is changed, unless "delay evuluation" is used, in which case it is necessary to press "evaluate sketch" to update it.
When it is finished then choose another view to be the active sketch view and the part navigator should now show the sketch as a child of the view in which it was drawn.
cowski (Mechanical)
1 Mar 10 13:23
Tom,
Thanks for posting your method. I have some drawings to do in the near future and it may come in handy.

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