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CAM profile in drafting

Phenom
Phenom

Hi,

on pippo_TAV1.prt I've add the CAM profile view using 'Layer visible in view' but I need to put entities in layer in master part, en extra work that I'd like avoid.

It's possible generate a solution like pluto_TAV1 using the reference component and flat-pattern#1 view.

I would like replicate the idea used for sheet metal part to add a special view that contain only the cam profile (SKETCH_000).

Attached some examples. 

Thank you...

Using NX 11 / RuleDesigner PDM

9 REPLIES

Re: CAM profile in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @cubalibre00,

 

Take a look at the attached.  I may have done too much, but essentially saved a new view in pippo, made the profile view dependent in that view (probably unneccesary), created a new Reference Set called CAM PROFILE and added only the sketch to that Reference Set.

You can now use the Add View of Part to add the CAM PROFILE view to pippo_TAV1, and then replace the reference set for that reference component to CAM PROFILE.

 

I think this is what you're looking for, but let us know otherwise.

Regards, Ben

Re: CAM profile in drafting

Phenom
Phenom

BenBroad wrote:

Hi @cubalibre00,

 

Take a look at the attached.  I may have done too much, but essentially saved a new view in pippo, made the profile view dependent in that view (probably unneccesary), created a new Reference Set called CAM PROFILE and added only the sketch to that Reference Set.

You can now use the Add View of Part to add the CAM PROFILE view to pippo_TAV1, and then replace the reference set for that reference component to CAM PROFILE.

 

I think this is what you're looking for, but let us know otherwise.

Regards, Ben


Hi Ben,

it's what I'm looking for, but Add View of Part is hidden on NX11 and grayed.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: CAM profile in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom

Not sure why it would be greyed out...

Open your "Menu > Insert > View > Base..."  dialog.

Right at the top of the Base View dialog is a block titled "Part" that is collapsed.  Click on it to see parts in your session.  Select "pippo.prt" to add views from that part ("Add View from Part").

Re: CAM profile in drafting

Phenom
Phenom

Hi Ben,

I'm tring to replicate your work, but nothing.

Attached a video.

Another question, in your cam profile view, you have hidden the body and I'm not able to revisualize. What have you do to hide the body ?

Thank you...

Using NX 11 / RuleDesigner PDM

Re: CAM profile in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom
Having placed the view, locate the drafting component in the ANT, right click it, and change the Reference Set to "CAM PROFILE". Of course, this is assuming that you made a Reference Set in pippo.prt called "CAM PROFILE" and removed the body from that reference set and added the sketch.

Re: CAM profile in drafting

Phenom
Phenom

Hi Ben,

sure I don't have see my video, because I used your file and deleted the view you have add to replicate what you have done.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: CAM profile in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @cubalibre00

 

Your part was created without the Customer Default "Create Drafting Component".  Therefore, having set the customer default and restarted NX, you must remove the existing component and start again.  As a result, you should see the drafting component icon in the ANT for the view added using View of Part along with the regular component icon for the master model (see attached).  That may explain why you cannot replicate my results.

 

Regards, Ben

 

Re: CAM profile in drafting

Phenom
Phenom

BenBroad wrote:

Hi @cubalibre00

 

Your part was created without the Customer Default "Create Drafting Component".  Therefore, having set the customer default and restarted NX, you must remove the existing component and start again.  As a result, you should see the drafting component icon in the ANT for the view added using View of Part along with the regular component icon for the master model (see attached).  That may explain why you cannot replicate my results.

 

Regards, Ben

 


Hi Ben,

I've set in the Customer Default "Create Drafting Component" and I'm able to replicate your workflow, but playing with this setting I've found some big limitation :

1) A "Drafting component" like an assembly will not be reported in parts lists.
2) A "Drafting component" cannot (Starting NX9) be substituted/ replaced.
3) A "derived views" works fine on drawing components but in case you want another base ( such as a TRI-view ) view you need to add the component again.
4) In case there are multiple "Drafting component" , it's not so simple identify which one is shown in which view. - There is no cross-highlighting.

 

After that, I ask to you, that are Siemens PLM employed, why I need to set this option in the customer default and if it's possible, explain me the description of this implementation.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: CAM profile in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom
I've set in the Customer Default "Create Drafting Component" and I'm able to replicate your workflow, but playing with this setting I've found some big limitation 

 

 

1) A "Drafting component" like an assembly will not be reported in parts lists.

Correct.  It is a view of a component - a reference view.  It is a visual representation to indicate that you had added a view of a component rather than a view at a higher level (pippo_TAV1).  It will not show any geometry added at the higher (pippo_TAV1) level.


2) A "Drafting component" cannot (Starting NX9) be substituted/ replaced.

Correct - by design.  It is not a true component, but a reference to a component.


3) A "derived views" works fine on drawing components but in case you want another base ( such as a TRI-view ) view you need to add the component again.

Not sure what you mean by this.  You can add a view from pippo_TAV1 (work part, no drafting component in ANT) or pippo (view of part, drafting component in ANT).  I had to remove and re-add the original component in order for the parent part to read the change in the customer defaults, the drafting component to show up in the ANT and allow you to choose a different Reference Set for that view in order to show ONLY the sketch.


4) In case there are multiple "Drafting component" , it's not so simple identify which one is shown in which view. - There is no cross-highlighting.

Multiple View of Parts of the same component only add a single Drafting Component to the ANT.  A View of Part of a different component will add a new Drafting Component.  Selecting a Drafting Component in the ANT highlights the geometry in the corresponding views.

 

After that, I ask to you, that are Siemens PLM employed, why I need to set this option in the customer default and if it's possible, explain me the description of this implementation.

 

This customer default provides a visual aid to determine whether a view has been added from a lower level component.  These types of view do not update to changes made at higher levels, so would aid in establishing whether a view that does not show new geometry is a view of part or not.  As I have demonstrated in this example, drafting components allow you to add views and use alternative Reference Sets to show geometry in the part (sketches, flat patterns, etc), rather than at a higher level (typically reserved for solid bodies).  Without this option you would have to add the sketch to the MODEL reference set and use layer masking to hide the body and show the sketch - but then that wouldn't replicate the flat pattern example that you asked the forum to reconstruct.

 

Regards, Ben