What is the easiest method to mirror complex 3D sketch?
I want mirror this sketch about the front plane.
Any help will be appreciated.
Unfortunatelty there is no easy way to do this as standard 2D sketch commands don't apply. You could always save the sketch as a part. Insert two of them into an assembly, orientate them accordingly and then save the file as a part file. There is a load of "dog-leg" techniques that may help such as: Video Tutorial on Mirror 3D sketch in SolidWorks Method #1 - YouTube . But in summary it is not easy unfortunately. Sorry I couldn't help more.
Create surfaces from your sketch, mirror the surfaces, then use the edges of the mirrored surfaces to create a 2nd 3d sketch?
Are you trying to mirror those lines so that you can make something? Could you just model what you want instead?
Yeah i want to mirror those lines.
Do you know how to make a plane at the end of a line that would be normal to that line? Select one of the lines and then select the endpoint of that line and then select the plane tool. This will give you something to mirror about.
You can try this.... (but really you really were offered good solutions) So now here is the long way outta round......
Save what you have as a part file... Open a "New" assembly file, insert the saved Sketch Part, Mate origin to origin, front plane to front plane, right plane to right plane, Save the Assembly. Open the Sketch Part, select the right plane and go to Insert/Mirror Part and save the Mirrored Part and close. Now go to the Assembly and insert the mirrored part, then mate origin to origin, front plane to front plane, right plane to right plane, save the assembly.
Now insert "New Component" and save, open a 3D sketch and then trace each line in both parts exit the sketch and save, now you have a part with mirrored 3D lines.....
I think it would be quicker picking any of the other ways
I will try.If it worked then it will be quickest method for doing so for me.
Thank you so much
Create the solids or surfaces for whatever you are modelling on the half you have, and then create the mirror.
Sure i did.
But that will give me solid body.
But i want line data both side
That could be a good idea. You could create your solid body, then convert the body edges to skech entities then hide the solid ody so it appears as if just skech lines are present.
I have converted those lines into pipes.
How will I convert the body edges to skech entities?
Start a sketch on a plane and select the model edge and convert the edge to a sketch line as above.
you can sketch a simple cross to do a swept surface along your entities
resulting in 2 surface bodies like so..
then mirror the two bodies about the plane
you can then do an intersection curve to quickly generate the opposite hand sketch. the intersection is between the two mirrored surface bodies.
hide or delete surface bodies.
Deleting the surface bodies will put a delete feature in the tree.
Yes, this may be the direction to take this. Though, one thing to keep in mind is how all of this works. When you use convert entities, the line segment ends are free to be dragged around at the line ends (I don't think this is the case where two line segments intersect). So, you need to be aware of that and make those end points coincident with those points. I'm sure there is some reason for this functionality, but it never made sense to me.
You have some good replies here. But, I'll throw my 2 cents in...What I have been doing in a similar circumstance is to recreate the sketch on the other side of the plane and join the two with a construction line with a center point relation on the plane, then make the line segments equal. It is more labor intensive than some of the other suggestions (2018 may fix this, but I wouldn't touch that with a 10 foot pole for production work). But, so far it is working. Though, I don't have as complex a sketches.
I think someone on these forums stated something to the effect that if you have more than something like 30 sketch relations you may be asking for trouble. So, it may be best to break it up to multiple sketches at 30 relations or so.
Looks like Matt Peneguy beat me to it, so this is basically just a re-hash of what he posted:
Something I've done before was to "show" the sketch I want to mirror and start a new 3D sketch. I would attach construction lines to the endpoints of the sketch I want to mirror, constrain them to be perpendicular to the plane you want to mirror across (if I want to mirror across the Front plane, then constrain them to be "along Z"), and make the midpoints of these construction lines coincident to the plane you want to mirror across. The endpoints of the construction lines should then represent mirrored endpoints of the original sketch, so you can manually draw a sketch that connects these endpoints and will be a "mirror" of the original.
Probably not the best way to go about this if your sketch is very complicated, but I figured I would offer it as an option.
Another option for you. Not the most convenient but workable
Apply symmetry relations
You can select your entire sketch, or chains of entities and CTRL drag them to create a copy then add the symmetry relation to each vertex
very good suggestion.
But in my case when I tried to CTRL drag then new sketch is created.
Then how will I select two points of different sketch?
If you drag the sketch from the tree you will get a new sketch. If this is what you want then you should still be able to apply the same procedure. Just edit the second sketch and apply your relatations.
If you are editing the first sketch and CTRL-drag sketch entities then you should get a copy in the same sketch
There's another option now - they've added a mirror 3D sketch tool in Solidworks 2018.
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