Cable without Cabling??

[JimiH]

Hi

We dont have the cabling option in our proe, I created the following using surfaces and the intersect command.



Its a bit of a pain to achieve plus I have to hide the extrudes and intersects to just display the section sweeps but when I open the part again it displays like below, so I have to hide them again.



Anyone have any easier methods of creating this or to ensure the hidden features dont display by default?


2009-07-02_082359_cab.zip

Thanks

Geoff

 

[dannerj]

Well, I'm not sure about an easier way to create that, but
I'd be interested in a possible solution as well. As far
as not displaying hidden items, after you hide, go to your
layers, and save status, then save your assembly/part/etc..
Next time you open, they should stay hidden.

 

[doronron1]

Have you tried creating a datum curve through points, then sweep a section ?

 

[TS3g]

You should be able to go to View>Visibility>Save Status (after you hid what you wanted) to make the hidden objects stay hidden if they aren't by default.

Or do like doronron1 said.

 

[jvidal]

Hello!

dannerj is right: go to View > Visibility > Save Status.

However, shouldn't you get the same result without the extrude features? I mean, create both sketches and then intersect them.

Plus: the original sketches will automatically be hidden.

Best regards!
JVidal

 

[kdem]

Here is a cable example with points if you decide to try and use this method.


2009-07-02_101048_cable_with_points.zip

 

[JimiH]

Thanks Guys the View > Visibility > Save Status worked a treat

I had a go of points method kdem seems long winded.

I'll stick to the intersect method

Thanks

Geoff

 

[zpaolo]

However, shouldn't you get the same result without the extrude features? I mean, create both sketches and then intersect them.

Definitely, that's the way I do it sometimes, it works well.

Paolo

 

[JimiH]

However, shouldn't you get the same result without the extrude features? I mean, create both sketches and then intersect them.



Plus: the original sketches will automatically be hidden.



Best regards!

JVidal

The sketches dont intersect though, there on different planes. Its only when you extrude the surfaces do they intersect each other.

thanks

Geoff

 

[JimiH]

Well I stand corrected it does work, so thats two extrudes deleted

Cant see how this could be done with any less mouse clicks.

Thanks Jvidal






Edited by: JimiH

 

[jvidal]

Glad I could help.

 

[kdem]

Thanks Guys the View > Visibility > Save Status worked a treat

I had a go of points method kdem seems long winded.

I'll stick to the intersect method

Thanks

Geoff

You can also just use the datum point feature which will give more flexibility than the Offset Coordinate System Datum Points since you can just drag the points. Or a combination of both. If you are going to place points on surfacesyou can place the points on the surface,specify offset references, and drag the points to locations using edit definition. Gets rid of the intersect features and one of the extrude surfaces and you can redefine the cable position by editing the definition of the points. Here is an updated example of your fileswith the points if you still want to experiment with it.


2009-07-02_121618_cable_with_points.zip

 

[zpaolo]

The sketches dont intersect though, there on different planes. Its only when you extrude the surfaces do they intersect each other.

But it's not necessary that the sketches touch each other, they should just be on orthogonal datum planes, you can "intersect" them and the result is the same as if you extruded and intersected the sketches. I must say the term "intersect" here is a little misleading

Paolo