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NX-6 Sketcher in drafting view
- Thread starter HerbC
- Start date
JohnRBaker
Mechanical
What you need to do first is to make sure that the 'Sketcher Tools' toolbar is active, so if it isn't go to Customize and turn it ON .
Once this toolbar is displayed you will notice that it looks very similar to what you would expect to see if you were in modeling and you had entered the Sketch task, only in NX 6.0 Drafting there is no need to enter the Sketch task since sketching is now considered a 'normal' activity.
When you have the Sketcher Tools toolbar active you will note that the first item on the toolbar probably says 'SHEET1' indicating that if you were to select one of the sketcher tools from the toolbar that you would be creating a sketch on the face of the Drawing sheet itself. However, if you wished to sketch in one of the drawing views, just go to this first item and select the desired view (you can also select the view, press MB3 and select the 'Active Sketch View' option, or you could also go to the Part Navigator which will allow you to access the sketches from the list of drawing views). Now when you select a sketcher tool that view will highlight and as you draw, your sketch curves will be added to only that view (don't worry about the view boundaries, since they will automatically adjust so that the sketch is always fully visible). When you are done sketching, you can select another view or return to the drawing sheet as a sort of default 'Home' position.
Once a sketch has been created in a view, if you wish to add to it or perform an edit, all that you have to do is either double-click any of the sketch curves or select the view from the Sketch Tools toolbar and that will become your active sketch once more. Note that there can only be ONE sketch per view as well as ONE sketch per drawing sheet.
This is a sort of an introduction to a concept which some people refer to as 'Sketch anytime' something which will also be offered as a Modeling option in a future release of NX.
Anyway, I hope this helps you understand how sketching works in NX 6.0 Drafting.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
Once this toolbar is displayed you will notice that it looks very similar to what you would expect to see if you were in modeling and you had entered the Sketch task, only in NX 6.0 Drafting there is no need to enter the Sketch task since sketching is now considered a 'normal' activity.
When you have the Sketcher Tools toolbar active you will note that the first item on the toolbar probably says 'SHEET1' indicating that if you were to select one of the sketcher tools from the toolbar that you would be creating a sketch on the face of the Drawing sheet itself. However, if you wished to sketch in one of the drawing views, just go to this first item and select the desired view (you can also select the view, press MB3 and select the 'Active Sketch View' option, or you could also go to the Part Navigator which will allow you to access the sketches from the list of drawing views). Now when you select a sketcher tool that view will highlight and as you draw, your sketch curves will be added to only that view (don't worry about the view boundaries, since they will automatically adjust so that the sketch is always fully visible). When you are done sketching, you can select another view or return to the drawing sheet as a sort of default 'Home' position.
Once a sketch has been created in a view, if you wish to add to it or perform an edit, all that you have to do is either double-click any of the sketch curves or select the view from the Sketch Tools toolbar and that will become your active sketch once more. Note that there can only be ONE sketch per view as well as ONE sketch per drawing sheet.
This is a sort of an introduction to a concept which some people refer to as 'Sketch anytime' something which will also be offered as a Modeling option in a future release of NX.
Anyway, I hope this helps you understand how sketching works in NX 6.0 Drafting.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
JohnRBaker
Mechanical
One slight correction. While you can only have one sketch per view. You can have multiple sketches on a single drawing sheet.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
- Thread starter
- #5
JohnRBaker
Mechanical
I did say that some people refer to this as 'Sketch anytime', although perhaps 'Sketch all-the-time' might have been a better description ;-)
That being said, there is NO 'Finish Sketch' icon. Just set the 'Sketch View' item back to 'SHEET1' or simply leave it as it is as it doesn't really matter.
And if you're concerned about the 'active sketch' appearance as seen on the screen, when performing any sort of Printing, Plotting, Exporting to PDF operation, these will all treat the 'sketch' as if it were simply curves added to a view and it's appearance will be the same as any 'inactive' sketches.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
That being said, there is NO 'Finish Sketch' icon. Just set the 'Sketch View' item back to 'SHEET1' or simply leave it as it is as it doesn't really matter.
And if you're concerned about the 'active sketch' appearance as seen on the screen, when performing any sort of Printing, Plotting, Exporting to PDF operation, these will all treat the 'sketch' as if it were simply curves added to a view and it's appearance will be the same as any 'inactive' sketches.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
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