Paste New question

[broncomech]

I need to copy a sketch to a new document but I can not get  paste new  to show up in any menu, only option is paste.

Does paste new work with sketches?

[TrippyLighting]

You cannot create instances of sketches. You can only create independent copies of them, which is why there is no distinction between paste and paste new for sketches.

You can only create instances of components, which is done by paste, and independent copies with paste new.

In fact you cannot really copy sketches, just sketch elements. You can export the component the sketch is in and insert it into the new design and then copy the sketch elements into a new sketch.

[broncomech]

Thank you.

 I am trying to wrap my head around the difference between components and sketch elements.

My guess is this: I draw a shape to use as a cutter, then draw square and extrude it to a cube, then extrude the first shape to cut the cube to a new shape.

My new shape is the component/new body and the first shape is an element/sketch?

My primary concern is not altering previous versions of the design I am working on as I may need to back up one or two versions at a later date.

[TrippyLighting · Accepted solution]

The first thing you need to understand is the difference between a body and a component.

Sketches can have several different uses, but most often they are used to create the base shape for a body.

Both the sketch and body created from it might live in a component.

To create a independent copy you can copy and then paste new that component.

To make sure everything is created in the component you should follow Fusion 360 R.U.L.E #1: Before doing anything, create a component and make sure it's activated.

For newly created components activation is automatic. Activating a component will ensure that all objects such as sketches, bodies, construction geometry its are created in that component.

[broncomech]

Thanks for the link, I have it bookmarked now.

[Anonymous]

One more thing to recognize is that you can create a part (file in your library) that is just a sketch and co-ordinate system with nothing else in it.  Then insert it into another part as a component.  Once its in there you can use that sketch to create geometry in the parent part file.  This is handy if you have a standard detail you use everywhere and want it to be the same (and update if you need to change it) in every part your model.

[Anonymous]

after some experimenting I found what I think is a bug.  A part added as a component, referenced by some other feature in the model, and then removed no longer updates in the parent model file.  To get the update to work, you have to roll the history back to before the remove operation.  It seems like that should work without the rollback.

 Example file here:  Parent part http://a360.co/1YyeO7W  Child part: http://a360.co/1ZXQISB

Eric

[broncomech]

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@Anonymous wrote:

One more thing to recognize is that you can create a part (file in your library) that is just a sketch and co-ordinate system with nothing else in it.  Then insert it into another part as a component.  Once its in there you can use that sketch to create geometry in the parent part file.

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Thank you Eric,

 This is exactly what I am attempting to do but I DO NOT want to update the donor file. I have also run into the issue of warnings being generated when deleting an object that was created

using the sketch as a cutting tool, my work around is to drag the unwanted item out of view and set it as invisible.

[Anonymous]

Use "remove" instead of "delete" to make the donor part go away.  If you don't want to update, just select the component and right click "Break link".  If you just want the sketch geometry and no connection to another file, it would be easy to bring in the sketch component, copy the contents, paste it into the a sketch in the parent part, and delete the component.

Hope that helps.

[broncomech]

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@Anonymous wrote:

Use "remove" instead of "delete" to make the donor part go away.  If you don't want to update, just select the component and right click "Break link".

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Thank you,

 I had never noticed the remove option before.

Looks like I have no components only Bodies in my sketch so as I understand it there are no links to break until I create a component.

[Anonymous]

Right, break links only applies to components

--
Eric T Peterson, P.E.
Managing Partner
Lagom IDEAS Llc
ph: 206 427 5442