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Are you sure its merge and not intersect? I've been able to find information on intersecting curves. As far as I know and have been able to find out, merge is used to join surfaces.
If you look at the help you do indeed see and Edit > Merge for curves,
however it seems to be for when you import a curve from another part or
something.
If you can do it for that, though, there must be some way to do it within one
part.
Anyway, at this point I would be content just knowing how to "splice" or
connect two spline curves in sketcher. Knowing that'd be enough to get this
thing I need to get done in the immediate term.
I finally found the option. It took a little while for me to figure out exactly how to get to the menus. The option only works with imported datum curves. As a starting point, take your part file with the datum curves, they don't have to be touching,and save a copy of the file as an *.igs file. Start a new part and start the datum curve feature. Use the From File option and import the *.igs file you created. It creates a single datum feature with the curves in them. Select the feature in the model tree right click>edit definition. The Redefine Menu opens up and curves will be selected and click done. You will then see the Edit Curves menu with the merge option.
To 'merge' a curve chain; Pick the chain or a lead segment then Edit -> Copy, Edit -> Paste.If you want a single curve (vs.a one feature chain) use Approximate. The component segments will have to beG1 minimum, I believe.
Look in Help / Part / Edit Features / Copy and Paste / Copying and Pasting Surfaces and Curves for more info.
to do this, just set the selection filter to geometry>select any curve or portion>copy>paste and click on refrences button on dash board, now click on the details button, now you are able to select as many connected curves as you like. When you finish the feature you will get a combined curve.
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