All,
I have a formed beam I would like to mirror in an assembly to avoid the work of forming the opposite bent part. I have mirrored it however the cuts in thelower side of the beam are mislocated as if the part were rolled over rather than mirrored. What am I doing wrong?
I am in Inventor 2012.
Thank you
Jim S
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Jim,
Haven't opened your models, but what I have found to this point is that the mirrored components are not constrained.
So if you just grab them they will move. I ended up grounding them in these cases.
Does this info help you? Probably not. But my suggestion would be to try and do the cut in the parts instead of in the assembly. If this is possible in your case.
Thank you Scott. The mirrored part was not constrained but that was not the problem. In the screen shot below you can see how my beam is bent and the other end is trimmed. When this is mirrored I get the effect that the beam is essentually rolled over rather than mirrored. See bottom picture. I used the plane between the two beams so I would expect the cuts to be reversed from how they came out.. I have mirrored the part in the part stage but it is not associtative with the part it came from like they were back in my Pro-E days. At this point I would just like to know how to make mirror work correctly for in the future.
Thank you
Jim,
What options did you use in the Mirror command in the assembly? The result you're showing isn't really what I would have expected either. The result you're showing looks more like a 180 degree circular pattern than a mirror to me.
There don't seem to be many options. In the assembly I select the part and then select mirror.
The only remaining input is for the mirror plane which I select the plane between the two beams. It is in the same place as the visable mid plane on the smaller connecting beam. It seems straight forward, but is not acting that way.
Jim
It looks like you selected to re-use the component rather than to create a new derived component. See the difference in the attached image.
Edit: To be more clear, the circle next to the filename in the mirror dialog needs to be the green one, not the yellow one. And in case you are colorblind, it needs to be the symbol with the opposite arrows, not the symbol with the plus.
@JimSteinmeyer wrote:I have mirrored the part in the part stage but it is not associtative with the part it came from
If you did a Derived Component mirror the mirrored part would be associative to the original.
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@cwhetten wrote:It looks like you selected to re-use the component rather than to create a new derived component. See the difference in the attached image.
Edit: To be more clear, the circle next to the filename in the mirror dialog needs to be the green one, not the yellow one. And in case you are colorblind, it needs to be the symbol with the opposite arrows, not the symbol with the plus.
Yep - that was the setting I was thinking of when I asked. What cwhetten is saying is correct.
To get a mirror image (left and right hand, etc) version of a part, rather than just two instances of the same one on opposite sides of the assembly, you should use the Mirror option. This creates a derived copy of the original, reflected about the mirror plane. With the option you selected, you are telling it to use an exact duplicate of your original part, rather than a mirror image.
Thank you guys, yet another mystery solved. I thought I had selected the green button the first time but apparently I did not.
JD, the next time I create a mirrored part I will look for icons that might allow me to make sure the part is derived, I didn't see anything this time but that doesn't mean it wasn't there.
Thank you every one.
@JimSteinmeyer wrote:Thank you guys, yet another mystery solved. I thought I had selected the green button the first time but apparently I did not.
JD, the next time I create a mirrored part I will look for icons that might allow me to make sure the part is derived, I didn't see anything this time but that doesn't mean it wasn't there.
Thank you every one.
The green button results in a derived component. It doesn't actually spell that out in its tooltip, but that's what it does.
Just be aware that if you mirror in an assembly Inv always uses the same plane and adjusts the rotation angle which is not editable.
This gets messy if you use a combination of normal and skeletal methods.
If you want to derive your mirrored part into another part it will be in the wrong position. To avoid this create the mirror part using derive and select the mirror option and correct plane so it can then be inserted into other parts and have the correct orientation.
If I understand you correctly, what you are saying is that if I derive the part using the assembly X-Y plane to mirror about and then place the derived part in a different assembly at a different angle to the X-Y plane the part will change, But if I mirror the part about a plane in the part for example, The part intered into a new assembly will behave as normal?
This is good information to know as I mirrored using the first method.
Thank you
Jim
I think you sort of got it. The part wont change, just its orientation.
When mirroring in an assembly inv always mirrors the part about its XY plane and then adjusts the rotation to get it in the right position. You can see this under iprops occurance tab. So if you mirror about the assembly XY plane then no problem. If you mirror about YZ or XZ then it will have problems deriving.
To fix the derive issue you can edit the derived feature in the mirrored part and change the mirror plane. But then in the assembly it will flip into the wrong position and you cant edit the angles, so you have to delete it from the assembly and re-insert it.
If you dont use skeletal methods it wont be a problem. But if you do then instead of using assembly mirror use derive at part level instead.
It will all make sense if you just do a quick model with a mirror about YZ and have a look at the iprops.
Also remember that when you mirror in an assembly no mates are created. Move the first part and the mirrored part doesnt move. You have to manually add mates.
Thank you for your assistance.
Jim