CATPart points

[Runz]

Can the points created within a CATPart be shown in the drawing views of the part model?

I have located and created points on the model that are to be used as the Datum target locations and want to be able to show them on the drawing views

Thanks

 

[Albigger]

As long as they are shown in the model and not hidden, then can be shown in the drawing.

On the drawing view, go into properties and check the box that says "3D Points" on the "View" tab.

-- Jay

 

[Runz]

I saw that option, but it was greyed out.

As you mentioned, the points are visible on my model, but they are not showing on my drawing views.


Thanks,

 

[Donnis]

They can be also "transfered" in the drawing: select the 3d points visible in your drawing's view, right-click on selection and choose "Duplicate geometry" (function similar to "SPC->DRW" in Catia V4).

Regards,
Conrad

 

[Runz]

It doesn't appear to be an available option. Not only is it greyed out in the view properties, but it is also greyed out in Options (Tools=>Options=>Mechanical Design=>Drafting=>View).

 

[nev99]

Try

Tools>Options>Mechanical Design>Drafting>View>Project 3D Points

Regards

Nev

 

[Azrael]

Are you using "Generative View Styles"??? Turn it off and you will be able to show points. Tools->Options->mechanical Design->Drafting->Administration tab, last one on the right. Toggle on to prevent usage of view style.

The only other necessity is that view generation mode is set to exact

 

[Runz]

In regards to Nev99 comment, I tried to check that option, but as mentioned above, it is greyed out and it can't be changed.

I also checked the settings that Azael mentioned and both were already set to Prevent Generative View Styles and exact mode.

Could it be something in the Standard? I logged in as administrator, but didn't seem to see anything that would cause this problem.

We are running R16 sp5

Thanks again for all the input!

 

[Azrael]

Then the only thing left I know of is to check in the property of the view if the view is locked. Locked view will not give you any options.

 

[Runz]

I had "Enable occlusion culling" checked (Turned on).

I unchecked the box and the "3D points" option becomes available.

I don't know what that setting is or why it was checked, but at least I found the problem.

Thanks again for all the replies!

 

[Azrael]

"Enable occlusion culling" works on solids only so that's why the wireframe didn't show. It's a setting so it don't calculate hidden solids, performance.... didn't think about that one.