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Mirror Feature In Solidworks

Discussion in 'DRAWING, LAYOUT & CAD' started by alloy, Jun 26, 2016.

  1. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Not much activity in this forum, but I thought I would ask anyway.

    I am taking a Solidworks class using 2015-2016 student software and have drawn a part that we are supposed to mirror. But I need to mirror and rotate the mirror. The instructor told us to use any resources we could come up with. Well, everyone here is a resource to me.

    Here is a screen shot of the file. It would be easy to just build the part from both sides, but where is the fun in that. The instructor knows how we made the part, so no fooling him on it.

    I would appreciate any help I can get. I am hoping to get my CSWA at the end of the class.




    bonus 1-3.PNG
     
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  2. MSD0

    MSD0 United States Active Member Active Member

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    Can you show the plane or face that your using to mirror the part?
     
  3. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    20160626_180239.jpg

    It is drawn on the top plane. I have a center line to mirror around.

    The pic above is what I am trying to achieve.
     
    Last edited: Jun 26, 2016
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  4. MSD0

    MSD0 United States Active Member Active Member

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    I don't have my computer in front of me to verify, but I think you can only mirror about a plane. If you select the top plane and mirror the part, you should have several options which control orientation:
    • Orientation 1: Translation over mirror plane, no rotations
    • Orientation 2: Translation over mirror plane, rotated 180 degrees about the Y-axis of the part file
    • Orientation 3: Translation over mirror plane, rotated 180 degrees about the X axis of the part file
    • Orientation 4: Translation over mirror plane, rotated 180 degrees about the Z axis of the part file
     
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  5. MSD0

    MSD0 United States Active Member Active Member

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    Should probably add that I'm using an older version of SolidWorks so might be different than the version your using.
     
  6. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Here is a screen shot of what choices are available to me. It may be that this is educational software and does not have the full features.

    features.PNG

    It is easy to mirror, just no option for rotation that I can see.

    mirror1.PNG
     
    Last edited: Jun 26, 2016
  7. MSD0

    MSD0 United States Active Member Active Member

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    You may need to create a vertical axis through the center of the part. In the "mirror/face plane" box, try selecting the top plane as well.
     
  8. MSD0

    MSD0 United States Active Member Active Member

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    If you haven't figured it out by tomorrow, I can play around with it at work (don't have SolidWorks at home).
     
  9. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Thank you for all your help. I have been looking for this answer since Friday, so I did my homework, but no answer to this. All my other homework has been pretty easy. We just finished the first week of class and I turned in my homework that is due by the end of week 4. This is a bonus part. I figure why hang back with all the others when I can move forward and hopefully learn even more.

    I created a constructi0n line on the right plane, but I do not have the option to mirror around it.
     
  10. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    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.

    6-26-2016 0003.jpg 6-26-2016 0002.jpg 6-26-2016 0001.jpg 6-26-2016 0000.jpg
     
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  11. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    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
     
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  12. sanddan

    sanddan Active User H-M Supporter-Premium

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    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.
     
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  13. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    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.
     
  14. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    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
     
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  15. metastable

    metastable Australia Swarf Registered Member

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    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.

    Sent from my SM-T532 using Tapatalk
     
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  16. RJSakowski

    RJSakowski H-M Supporter - Premium Content H-M Supporter-Premium

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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.
     
  17. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    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.
     
  18. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    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!
     
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  19. sanddan

    sanddan Active User H-M Supporter-Premium

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    Well said petertha.
     
  20. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    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
     
  21. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    I think the mirror command is pretty straightforward in this case:
    - make a plane through center of middle square section (1)
    - mirror the add-on wedge section plus any of the subsequent pocketing features you created (2). Note you need to 'add' these collective features to the appropriate window.
    Some screen grabs
     

    Attached Files:

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  22. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Thank you.

    It shows how new I am, I was trying to mirror around a center line and couldn't get that to work.

    I'm learning, sometimes I'm pretty dense though.
     
    Last edited: Jul 3, 2016
  23. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    Keep up the good work. Everyone who uses SW was at your learning stage at some point or another (me included!).

    When you are dealing with 3D parts & features, mirroring typically involves defining some sort of plane to act as reflecting surface. It can be an XYZ origin plane or a plane which you have constructed from combinations of points & lines, or even the face of an existing part. An axis is an infinite line, so it lends itself to rotating or copying features about it. You cant 'project' an image off a line the way you can a plane.

    Where mirroring is somewhat ambiguous is inside a sketch. Here you are allowed to mirror a feature about an axis. Wait, we said an axis is a line (as opposed to a plane), which appears to break the rule. But this is a special circumstance because inside a sketch you are confined to 2D space. Specifically the plane you are sketching on is fully defined & everything in that sketch occurs on this same plane. So behind the scenes, the program can solve this mirror command in the context of 2D. I guess you could say the 'equivalent plane' is known because its always the axis line projected 90-deg perpendicular to the known sketching plane.

    I suspect this 'mirroring' terminology might be hangover from 2D days. And of course, we use 2D as the initial step in SW to eventually build 3D parts. But once we are in 3D space & now need to precisely make reflections or copies of 3D features, we need more rigorous definitions. I'm no expert, but this is about the best I can describe it.
     
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  24. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Our instructor touched on using a temporary axis but we haven't used one yet. It's funny how you can work for hours and not get it, and one little suggestion solves it.

    After I get a handle on Solidworks then I need to learn HSMworks. We have it at work and soon I'll have my CNC mill home and need to be able to program it. I have a lot of parts I want to make. I go to old car swap meets with my transmission mods and I always get people asking me to make parts. I've looked at some of the parts that they are talking about and there is an insane markup on them. A $50 piece on aluminum and 30 minutes on a mill and they get $395.

    Anyway here is the finished part I was working on, and the next one I did.

    Capture407024.PNG 4260192.PNG
     
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  25. petertha

    petertha Canada H-M Supporter - Premium Content H-M Supporter-Premium

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    I am green with envy.
     
  26. metastable

    metastable Australia Swarf Registered Member

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    One small tip: it is usually very convenient to set the origin up at the center of the part. This way you can use the origin and the principal planes for various things. In this case as a mirrior plane. This good modelling practice has 1001 benefits besides mirroring but it may become a hindrance every now and then (design intent).
    I am not sure about the latest situation but SW doesn't like to mirror some features (i guess chamfer didn't work). But in your case you should be able do it. When you want to mirror multiple features it is a good idea to pick team from the tree while holding ctrl. Then click on the mirror command and pick the mirror plane. In this case if you dont have a mirror plane (or surface) you should create one first.

    Sent from my SM-T532 using Tapatalk
     
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  27. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    We are using origin for a center of sketches as much as possible. Also construction lines. I learned last night how to turn a line into a construction line.

    Yes it doesn't like to mirror some features such as fillets and lettering. I was trying to circular pattern a logo but it just didn't work. I may ask about that tomorrow night. I also tried using polygon to make one lung nut On my wheel below, but couldn't make it do a circular pattern either.

    As I said earlier we are making Legos. We were doing revolve last night. Was very easy since I've been doing that for a couple of months now. I decided that I didn't want just a regular Lego wheel, so I made up my own custom version. Not sure how he will like that, but oh well. Was fun. I just learned tonight how to apply colors to different features. Below is my cool version of a Lego wheel. I "loosely" patterned it after the iconic Cragar S/S wheel :) cragarss.PNG
     
    Last edited: Jul 7, 2016
  28. Wreck™Wreck

    Wreck™Wreck United States Active User H-M Supporter-Premium

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    Correct me if I am wrong but that appears to be a symmectrical part which would by definition have no hand, this would make it a mirror of itself.

    I must be missing something, the drawings contain no dimensions in order to distinguish any features that gives them a hand either LH or RH.

    If, as it appears the instructor wanted you to merely mirror a single feature of the part and move it 180 Deg. in 2 dimensions on the other end in a 3D rendering then it makes a certain amount of sense as a training aid. If you get a job doing this remember that a majority of companies include a 3D rendering as an aid in visualizing what the part looks like for the person that must make it, a machine shop will not just post it in cam and run the machine from the generated code as this is entirely to risky.

    In 10-20 years this may become common, I expect to be retired by then, my advice would be to keep your drawings clean meaning no hidden lines or breaks that you can not see on the screen yet a cam system will simply stop when it gets there, it does not use the screen drawing but the data points from the cad drawing file. Do not have any unseen data points.

    Good Luck
     
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  29. countryguy

    countryguy United States Active User Active Member

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    Learned a ton on this one! Good stuff. Thanks! JJ
     
  30. alloy

    alloy Always looking for the next tool score H-M Supporter-Premium

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    Finished my mid term. Took a couple of hours to draw the 5 parts then assemble them. Thankfully there were no errors.

    One unfortunate thing I found out on Thursday is the advanced class may be cancelled. Apparently not enough intro students signed up for the advanced class. Really sucks, it will be 6 months before the advanced class will be offered and it's a 3 month class. Only one night per week.

    mid_term_assembly.jpg
     
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