Publish part axis

[jhsompura]

Hello,
I have created a simple revolve/shaft. The axis is defined in sketch. I want to publish its axis but the mouse does not point on axis. How can i publish the axis.
regards,
jiten

 

[MrCATIA]

Output Feature

An axis inside a sketch is just like a construction line - it is only usable within the sketch and is not available outside the sketch.

Unless you make it an "Output feature"

Edit the sketch, and right-click on the axis line and then select the option Output Feature. Exit the sketch. Now you can publish the axis line, by selecting it in the tree. It's hidden in the tree under the sketch branch in a sub-branch called "Outputs." Don't forget to rename the published line.

 

[MrCATIA]

Better Solution

Of course you want to follow your company's Best Practices. But before you publish the sketch axis, you might want to make a couple changes to how your CATPart is organized.

Since this axis line being used to drive several features, it would be a good idea to create it first, and rename it as the "blah blah centerline." You might want to group it into a special Geometric Set containing all the "master geometry." (this way it is easily identifed and not hidden inside of a sketch)

Then you can easily publish it for use in other parts.

The revolved feature can be defined with a sketch where the centerline is projected into the sketch and converted into the sketch axis, similar to what you currently have.

The objective is efficiency by having "master driving geometry" that is linked to many features. Changes made to the master geometry are passed down through the design to all the effected children parts and features.

 

[MrCATIA]

Another approach

Jiten, going back to your original post (and after doing a little investigation), I discovered you can directly publish the axis of a circular feature.

First, make sure you have Tool + Options set. Go to Infrastructure + Part Infrastructure, and in the General tabpage, make sure you have the option turned on for Publish a Face, Edge, Axis, Vertex, or Extremity.

Second, when attempting to select the revolved face to display the axis, use the Curve Filter option in the User Selection Filter toolbar.

I hope one of my three responses directly solves your problem, Jiten. If not, or if you need more help, please add a reply.

 

[jhsompura]

hello mr catia,
thanks for ur reply and interest.
i agree on ur second method and that does solve my problem.
but i am interested in other method as axis published in case of nuts and pins in mechanical standards catalog provided with other method.
i tried the first suggestion,i am working in R10 and on right click there is no ouput feature. Maybe a feature with upgraded version,dont know?
in case of the third one the user selection feature remains disabled. any advice to enable it?
eagerly waiting for ur reply.
regards,
Jiten

 

[MrCATIA]

Jiten, I'm sorry but I don't have any records of R10. That was about 5 years ago! You really should upgrade to R16 and take advantage of lots of new features.

Maybe someone else who is more familiar with R10 can tell us if Output Feature can be done with that release. It's a handy feature that I use often.

The User Selection Filter toolbar should be active when you're working in the Part Design or Shape Design workbenches. I'm not sure why your toolbar is inactive.

 

[jhsompura]

hi,
i believe axis can be published with out output-feature
i initialised a mechanical fastners bolts,nuts,pins..... from catalog.it has one face and its axis published I wonder how did they do it.may be u can try this hint and get something for me.
regards,
jiten.

 

[flanakins]

Here is a quick and easy solution.

Open Publication using Drop down "Tools"
Make sure that "Publish a face, edge, axis , vertex or extremity" is active
Right Mouse klick on our Cylinder.
Go to "Other selection"
Pick "Axis" from Menu
Axis appears in Publication box
Exit Publication box with "OK"
Axis is published.

 

[jhsompura]

Unbelievable I couldnt think such its working
Such a stupid of me.

thanks for ur replies both of u.
Regards,
Jiten.

 

[MrCATIA]

Thanks Flanakins - that is an easy solution (and a good tip)!