Mirror question 1

[jack3108]

Sorry to ask, but I need help:

I have a bracket welded from several plates. The plates are separate items - It_A.sldprt, It_B.sldprt, ... and so on.

The bracket is an assy of the parts.

How do I produce a mirror bracket in such a way, that if after MIRROR I add another plate to (LEFT HAND) bracket, it will automatically propagate to the MIRROR'ed (RIGHT HAND) bracket.

 

[ctopher]

Go to your Feature toolbar, then mirror component. Have a plane or surface to mirror with.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[jack3108]

This is not what I want - bacause if I add another plate to bracket I will have to mirror that plate ("manualy") and "re-adjust" configurations.

I tried to make next (higher) assy of LEFT hand bracket and mirror it on that higher assy (as a one item).

It does not work - it works but then if I add another plate to the lower assy (LEFT hand), on the higher assy only the LEFT hand get properly up-dated (that is, the added plate shows up). The Mirrored (RIGHT hand) part does not have that new plate.

Any idea where I am messing the things up ??

 

[MadMango]

The Mirror Part function as you are describing it only works for parts, not assemblies. Is there any way you can redesign your bracket to make it from one sheet metal piece? If so, then you could use the Mirror Part function.

If you can't, then you have to use Mirror by control-selecting your components (that make your bracket) you wish to mirror in your assy. It's easy enough to Edit Definition to add other component to the Mirror feature in the Feature Manger.

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[rgrayclamps]

You should create your weldment part using part model with multi-bodies instead of an assembly model.

Alex

 

[jack3108]

rgrayclamps ...


Thaks, it works

 

[jack3108]

Now I have another problem - on Extrude1 I placed Extrude2 (that is "Plate1" and "Plate2")

I need to have separate detail dwgs of Plate1 and Plate2.

If I Hide or Suppress Plate1 (so on the dwg I would have Plate2 only) both "plates" (atually Extrude1 and Extrude2) disappear - probably because Extrude2 can not exist without Extrude1.

Is there anyway around this - or what am I doing wrong?

 

[WorkingLife]

The easiest way (which is what I do) is to delete the body in your part. To do this, you must make sure that Extrude2 is not merged with Extrude1. So that in this case (I am simplifying it), you will have these four features on your design tree "Extrude1", "Extrude2", "Delete-body1" and "Delete-body2" as well as 2 configurations "Plate1" and "Plate2". Depending on which plate you want to see, you will suppress one of the Delete-Body function.

To delete the body, you have to access the solidbody folder and right mouse click on one of the listed item and select "delete body".

Then in your drawing, by selecting the correct configuration, you will have the plate that you want to dimension in that drawing view.

Hopefully this will work.

 

[jack3108]

WorkingLife [.....]

Yes man, I just discovered it the hard way - thanks for reply anyway.

My misteake was that Merge box was checked.

Thanks again to all replies !!

 

[jack3108]

Actually - still not what I wanted.

If I later add another Extrude ("Plate") to the part, it will show up on detail drawing of oanother part ...

The real solution would be (I think) what I intended originally - that is build the welded LEFT HAND bracket as an assy of indiwidual parts.

Then make higher assy where I bring in the lower assy. On that higher assy make MIRROR, and two configurations - LEFT and RIGHT.

Then you can use either LEFT or RIGHT assy for bracket assy drawings (manufacturing dwgs) or for that matter for machine assy.

Individual "Flame cut dwgs" for individual plates will not be affected, since they are made from individual parts.

Any added plate on first level bracket assy would show up on the next ("LEFT and RIGHT") assy - the catch is that the MIRRORED version does NOT show up the additional plate.

 

[jack3108]

Actually, I think it should be called BUG - because MIRROR does NOT beheave "dynamically", that is does not update the MIRRORed assy on the next higher assy the next time around the (higher) assy is displayed. I tried Ctrl-Q and "Rebuilt" icon - does not help

 

[rgrayclamps]

Hi, Jack3108:

It seems that you are confused with parts and bodies. In your case, you have only one part, which is the weldment part.

SolidWorks used to use assembly to model weldment parts. But the problem is that you need to create weld bead part(s) for your assembly. So, SolidWorks abandoned using assembly technique to model weldments (I do not remember since what version). You should use a multi-body part together with weldment cutlist for your weldment.

Alex

 

[jack3108]

Not so - the fact that I have a welded bracket has nothing to do with weldments.

Mayby I used wrong terminology - forget about the welds - imagine that those individual plates are magnetic and are held together with magnetic forces - no welds, no glue whatsoever.

Now, this is an ASSEMBLY of individual parts.

And I would like to MIRROR an assy.

And when I add or substract a part to/from assy (parent) I would also like to see the change in MIRRORed ("child") assy.

So far it does not happens. Once MIRRORed, the MIRRORED (Child) does not react to changes in "Parent"

 

[rgrayclamps]

I do not have good solution for your. But, mirroring an sub-assembly is not a good idea. It violates SolidWorks' basic foundation. You should built your parts individually, being it left version or right version. If you want to tie your left version part to right version part, you can always use "Derived part". Personally, I decided never to use "Mirror command" for parts, let alone assemblies.

Sorry I can not help you.

Alex

 

[mkmech]

Hello rgrayclamps

I was just reading this post out of curiosity...

Can you elaborate what you mean by "mirroring an sub-assembly is not a good idea. It violates SolidWorks' basic foundation."?

Also, if I build separate right and left versions of the parts, how do I place them opposite to each other without having to use several mates? Mirror seemed like an easier way to do this but doesn't look like it works.

Thanks

 

[rgrayclamps]

Hi, Mkmech,

SolidWorks is an object oriented program based on database. It works best when you treat each part or assembly independently as an object. A part is an object in SolidWorks, so is an assembly. When you try to mirror an assembly, you are really thinking to mirror an assembly object without creating additional part objects for mirrored parts. It causes conflicts between parts and their assembly.

Based on this, a mirrored part is not good for SolidWorks (although the program allows it). Also, a part with multi-configurations is not good. Both of these methods create tangled objects (or parts). If you are familar with database, there is a basic requirement for database, which is "Normalization". By creating tangled parts (mirrored parts, parts with multiple configurations, for example), you destory this "Normalization".

Alex

 

[jevoltin]

If I understand what you are trying to do, I don't believe it is possible within SolidWorks. Each time you add a part to an assembly, you will have to manually initiate the mirror operation through one of several approaches. Otherwise, the new part would have to be incorporated into an existing (and previously mirrored) part, not just put into an assembly. If you combine the new part into an existing mirrored part through an operation like Join, the dynamic mirroring you desire would be possible. Unfortunately, I suspect that the effort required to use and maintain such an approach will be greater than simply mirroring each new part you create either separately or within the context of an assembly.

 

[mkmech]

rgrayclamps

Thanks for the explanation. However, when you say " When you try to mirror an assembly, you are really thinking to mirror an assembly object without creating additional part objects for mirrored parts, I get to think that SW DOES create mirrored parts (objects) when it mirrors an assembly, if we forget the dynamic mirroring question for a minute. Doesn't it?