No Share Sketch Option

[Vagulus]

I have created a Part in an assembly so that I can copy a spline curve and its relative position.

Construction Assembly 1

After extruding the crossmember (gold colour) I want to do another extrusion but I do not have the option to share the sketch.  AI2018 keeps telling me that I need a 2D Sketch to extrude from.

No Extrusion Option

Why is that and how do I get to share the sketch.

Thanks

[Xun.Zhang]

Hello @Vagulus,

Only one of property for sketch adaptive and sharing can be supported for a sketch node.

In this case, suggest to copy the sketch and paste to create a new sketch for sharing purpose.

Here is the idea to support this case in the ideastation, please cast your vote.

Hope it helps!

[Vagulus]

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@Xun.Zhang wrote:

Hello @Vagulus,

Only one of property for sketch adaptive and sharing can be supported for a sketch node.

I don't know what this says.  I do not understand what you are telling me.  I am just a 'Bear of very little brain' and I am afraid you will have to send me a link to some explanation of this.

In this case, suggest to copy the sketch and paste to create a new sketch for sharing purpose.

If I 'Copy' the sketch in the assembly, where and into what do I 'Paste'  it.  If I create a new sketch I cannot find a 'paste' option.

Here is the idea to support this case in the ideastation, please cast your vote.

Hope it helps!

This link leads to someone making a suggestion and someone responding to that suggestion.  I don't see anything practical here.

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[Vagulus]

There was a bit of confusion at my end.  I was 'Copying' a part, not a sketch.  Sorry about that.  Okay, now I have a sketch in the assembly and I can copy it.  How, and into where or what, do I paste it?

[Xun.Zhang · Accepted solution]

Hello @Vagulus,

Select a plane/face/workplace and then paste. that's all.

Thanks!

[Vagulus]

Thanks for that.

Like everything else, it's easy when you know how.  Pasting the sketch onto a plane in the new part is the key.

[jrohit1110]

Most Basic command. Not working that too in the 2021 version. Trash. Better use Fusion 360. 

@Vagulus I've been projecting sketch entities onto another overlapping sketch, but that's absolutely stupid. @Xun.Zhang please highlight this problem to Inventor developers at Autodesk. Also, if we search "Shared Sketch" in the Search command toolbar, we cannot find it.

[jrohit1110]

@Vagulus 
I may have found the solution (At least that's what worked for me) I don't really think that it's the solution, probably a  bug meh.... So, here's what you do>..........

1. I noticed that you've turned on 'Adaptive' for all features. You can go and change that in the Applications menu>>>

 Tools>Application Options> Assembly> "Features are initially adaptive" [Turn it off]

Hit 'Apply' and 'Close'

You can then see the shared sketch option when you right-click on the sketch in your design browser. 

Let me know if it works for you.

[johnsonshiue]

Hi! Adaptive was designed to link geometry from one part to another part. It can be used when dimensions are not clearly defined. But, it should not be over-used. When you need to establish Adaptive relationship repeatedly, you may want to look into different modeling approach: Multi-Solid Body or Derive.

You will define geometric relationship between different components within a part by creating different solid bodies. Once you are happen with the geometry, you can push individual bodies as parts in an assembly.

Another approach to consider is to use Copy Object. When you edit a part in place, you can use Copy Object command to link the body geometry from another part. This will allow you to project faces or edges multiple time. When the source body geometry changes, the adaptive part will update accordingly.

Many thanks!