Sketch application in drafting 3

[tomstickland]

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:

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]

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]

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]

Tom,
Thanks for posting your method. I have some drawings to do in the near future and it may come in handy.