Constraining a line to the edge of the model 1

[Gokulkrishna]

Hi,

I'm unable to constrain a line to be colinier to the edge of a cylinder previously extruded even after trying the different filters.

Even (in drafting enviornment) while inserting the base view the cylinder (side view --> circular end), entered the Active sketch mode and drew a cirlce. I can't set this sketched circular profile to be concentric with the cirular edge of the cylinder.

Thanx,
Gokulkrishna Goli
NX8.5

 

[JohnRBaker]

Why are you creating what appears to be construction curves while in Drafting?

Also, your image does not provide enough information for me to tell exactly what it is that you're attempting to do. Please either provide the actual model or a MUCH better picture of what you're trying to do.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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[Gokulkrishna]

Hi,

Please find the model. When we edit the sketch 2, the line 1 should be collinear with the edge marked in red(attached snap) and line 2 should be collinear with the edge marked in green.

Also if you enter the drafting enviornment of this particular model, I drew a arc and made it concentric with the circular edge of the cylinder. Now how to make these two curves coincident.

I want to show a no stampimg zone my drawing, please see the attached snap untitled 2.

Thanx
Gokulkrishna Goli
NX8.5

 

[JohnRBaker]

How about this approach (see attached model)? You can't actually use what you've show as the Green and Red curves since the are NOT real curves. What I did was create a point in the Model sketch where the edge of the cylinder intersected the plane of the sketch and then constrained the corner of your sketch (where line 1 and 2 come together) to be coincident with this point.

Then in the Sketch in the Drawing I projected the edge of the cylinder into the sketch and then constrained it to pass through that same point as above. Then I constrained your arc segment to have the same radius as the projected arc. I then created an offset curve plus two additional curves to define your 'no stamping zone'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Gokulkrishna]

Hi John,

Your approach is working fine till I have a single file for both the model and the drawing. But when I make a seperate file for the drawing and then link it to the model this intersection point is not visible.

We have to prepare seperate drawing files as there will be 3-4 part file created through the part families table. So I've to prepare seperate drawing file for seperate child file.

I have attached a model of the boss and a snap shot of the drawing file created seperately without the intersection point. Is there some setting to make this point visible?

Thanx
Gokulkrishna Goli
NX8.5

 

[JohnRBaker]

I'm not able to open the .prt file.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

It appears that a comma was added to the end of the part name which is messing up the download link. If you copy the link location, paste it into your browser address field, and remove the comma, it will download correctly.

www.nxjournaling.com

 

[JohnRBaker]

Have you edited the Model Reference Set so as to include the Point as well as the solid?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Gokulkrishna]

Hi John,

While inserting the base view in a drawing template I couldn't find the reference set option which is there while adding a component in assemblies. Could you inform me how to do that?

Thanx
Gokulkrishna Goli

 

[cowski]

Reference sets act as a filter for component geometry and are not used directly when creating views. A drawing view will show all of the filtered geometry for a given component (the currently used reference set); if the reference set is changed the drawing view(s) will update accordingly. You cannot have views showing different reference sets of a single component.

However, there are cases where we want to show multiple reference sets of a single component on a drawing... Let's assume there are 2 reference sets (A and B) that I want to show on a single drawing.

One option is to add the component twice, using ref set A for one instance and ref set B for the other. After adding a view, we can then hide one of the components in that view (there are multiple ways to accomplish this, probably the best is "hide component in view").

There may be better options depending on your end goals...

www.nxjournaling.com

 

[JohnRBaker]

The Reference Set is not per view, it's only when adding a Component, but it can be changed after it's added by going to the Assembly Navigator, selecting the Component of interest, pressing MB3 and selecting the Reference Set option which will show you not only the current Reference Set (it's grayed-out) but the list of available ones as well.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.