Target Points in drawing 1

[CPaul]

I would like the place a target point in my drawing view and be able to set the dimension (.060).
Looking at the help files, target points are not associative to model geometry, so how would I do something like this?
Also, when dimensioning the targets, the dimensions are off. I'm thinking this is because of the scale factor for the particular view?

Thanks in advance,
Chris

 

[CPaul]

sorry that picture is really large, here is a better version.

 

[jerry1423]

Is the target point just something in space, or is it asssociated to something on the model?
To me it doesn't look like it's associated to anything on the model.

 

[CPaul]

its a target in space, that I would like to dimension off featurs on the part.

 

[JohnRBaker]

If what you're attempting to do is to place a Target Point Symbol at some SPECIFIC location relative to some aspect of your model, as seen in a particular view, try this:

Go to...

Insert -> Curve/Points -> Point...

...and using the Offset option, create a Point located relative to what you wish to reference at the location where you with the Target Point to be. Then using the Target Point Symbol function select this point as it's 'Location'. Now just Hide the original Point and you should be good to go.

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.

 

[CPaul]

That was helpful, thanks John.

Another question.
After I get the point in there and place the target on it I put the dimensions in and they are off by the scale factor (supposed to be .060 but ends up being .240 because of a scale factor 4:1 in the view). Is there a scaling option I'm missing?

 

[CPaul]

*edit*

vertical dimensions are corret, horizontal dimensions are not.

 

[CPaul]

edit* again sorry.

some dimensions are off, some aren't.

 

[JohnRBaker]

If you're Views are not 1:1 scale, then you will need to select the View where you wish to place the Target Point Symbol, press MB3 and toggle ON the 'Expand' option. Then create the reference Point and the Target Point Symbol, Hide the reference Point. Now reselect the View, press MB3 and toggle OFF the 'Expand' option. Now you can finish dimensioning your Drawing.

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.

 

[CPaul]

it appears that I cannot create a point when in expanded member view

 

[JohnRBaker]

I just did it a minute ago. What version of NX are you running?

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.

 

[CPaul]

nx 7.0

I right click the view, select expand member view, and my sketch tools toolbar becomes grayed out.

 

[JohnRBaker]

Why worry about sketching if all you're doing is creating a single Point?

But if you insist, go ahead and create your Point using the 'Active Sketch View' approach, THEN Expand your view, place the Target Point Symbol, un-Expand the view and create your dimension.

In reality, it's NOT the Point that needs to be explicitly created inside the non-1:1 scale view, but rather the Target Point Symbol that needs to be located there to get the expected dimension.

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.

 

[CPaul]

How else would I put the point in the expanded view? I thought I needed sketching available in order to put a point in the expanded member view.

 

[JohnRBaker]

I explained how to do exactly that in my first post in this thread.

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]

Actually it's a combination of my first and second post which covers creating a non-sketch point in an Expanded view.

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.

 

[wecurb]

CPaul you are right, the pull down menues do not work (NX6). Open the CURVE Menu itself. Then you can add the required geometry in the expanded view. I had this same argument with my CAD support group. Their claim was that the pull-downs were not broke, my question was, "Why the different functionality???"

 

[CPaul]

John, I understand your steps but when I am in the expanded view, and go to insert -> datum/point, point is grayed out and I am not able to select it.

 

[JohnRBaker]

OK then, sketch the point in the view while working from the drawing and then expand it to add the Target Point Symbol, as only the symbol needs to actually be created in the non-1:1 scaled view for you to get the correct dimension value.

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.

 

[CPaul]

weird, but now when i sketch the point and target the dimensions are correct.