Mirror Feature In Solidworks

Just to show circular pattern works on multiple features more like your example (a circular boss and a separate rectangular boss).

6-26-2016 0004.jpg
 
Hmm...I'm just a hobby SW user but I cannot see a way to (1-step) mirror that topside feature to the opposing underside like that. Mostly because I can't envision a plane that would satisfy how mirroring works. So I'm going to chock this one up to A) my inexperience B) 'trick question' :) I do have a solution but its not mirroring, its a circular pattern. Here are the screen grabs FWIW.
- make an axis between 2 planes
- invoke circular pattern of the desired feature using this axis
- specify 4 pattern instances & delete the offending 2
- you are left with a single instance something like your desired end result

Hope this helps. Make sure & tell me what the answer is so I don't die without ever knowing.

View attachment 131458 View attachment 131459 View attachment 131460 View attachment 131461

That's how I'd do it.

Let me know if you need any help with your class. I used SW daily for about 8 years at my last job (before retirement) at Crimson Trace and about 15 years using ProE before that so I have a lot of cad experience. I'm just across the river from you in the Damascus area.
 
I'll give it a try again tonight and let you know.

Thanks everyone.

Thank you for your generous offer sanddan.
I may take you up on it at some point.

After I get a handle on Solidworks my next hurtle is learning HSMworks. I programmed for 15 years on smartcam but it's a whole new ballgame now. Since HSM runs inside Solidworks my plan is to get a good basic knowledge of solidworks before moving on to HSM.
 
Ok got it. I mirrored the part, but I unchecked merge bodies. That left the mirror free to move. Then I created a center line, went to circular pattern and copied it, and then deleted the the first mirror. Worked pretty good. Took a few tries to figure out what parameters to use. but it came out great.

Thank all of you for your help!

Now I will work on week 5 homework and take a look at my mid term final. Pretty sure I am able do that now with what I already know.

bonus 1-3.PNG l
 
Hi,

As a very experienced user i can tell that peter's way is the best way to go about this.

That being said, mirror command mirrors "something" accross one plane. In order to achive the transformation you need with mirror command you need to:

Either, create a new plane at an angle (probably 45 degrees but not %100 sure) then mirror about that plane.

Or, create the original feature as a seperate body and mirror it twice, delete unwanted body with delete body command then join three bodies with join command. This is not a very elegant way of doing it.

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Great to see that you have found a solution. That's the fun of using SW.

I believe that your method would not allow you to perform subsequent operations such as adding fillets though.

Another method would be to create the duplicated features as separate parts and put them together in an assembly and save the assembly as a part, if you wish. Not the most elegant way either but it would be useful if you had some complex orientation of the duplicated features.
 
We haven't done assembly yet so I didn't try that. I think assembly is in the advanced class. That's 4 weeks away.

I did radius the outside of the bosses and the support, along with the part profile and chamfered the ID on the bores before mirroring, you can see that on the left side bottom on the pic. But it apparently didn't follow to the top right boss and support when I mirrored it. But it did follow to the short boss on the left side. Until you mentioned it I didn't see that. I wonder why it did that?

In class tonight I will try and add the radius and chamfer. I may also take my final tonight so I can move on. At this point the class is on the line command.
 
I mirrored the part, but I unchecked merge bodies. That left the mirror free to move. Then I created a center line, went to circular pattern and copied it, and then deleted the the first mirror. View attachment 131497 l

You will probably hear the words 'design intent' about a million times in SW or parametric modelers in general. This might serve as a good example. If there is more than one way to accomplish an end result, always try & consider what would give you the most utility if you had to go back in & modify the part one day. Or if someone inherited your file & was trying to figure out what was done & why from scratch. The way I would interpret this exercise is you have a collection of sub-features on one side and you want this collection replicated identically on the other side. If the features needed to change for whatever reason, those changesit simply gets replicated to the other side.

Don't take this the wrong way but I think you are contorting 'mirroring' into a workaround of what is fundamentally a 'copying' operation. Checking merged bodies on/off doesn't really 'leave the mirror free to move', it just creates another unconstrained body in free floating space until you transpose into position by whatever means. In fact, lets say you have a very complex non-symmetrical base part & there was no convenient axis to do the circular pattern trick. That would be a perfect application for copying the (un-merged) seed body & then positioning copy(s) to where they need to be. Bodies are another one of those weird at first but potentially very useful aspects of SW. Happy learning!
 
I have another mirror feature question.

In my class we make Legos and at the end of the class we assemble them.

I'm making Lego #4260192. I have the one feature on the right side made, but can't seem to figure out a way to mirror it.

Any suggestions?

#4260192
24490-extra.jpg
And this is what I have now. Everything to the right of the center line are added features to the main block. The block was a separate part. I added the extrusion on the right side and did the extrude cuts down to the depth I needed.

I would like to mirror the right side "triangle" extrusion and extruded cuts to the left side if possible.

lego 4260192.PNG
 
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