I'm very new to Solidworks so this might be a simple problem on my part. What I want to do is mirror the tab shown below about the 'Right Plane' so I have an identical tab on the opposite side of the part. However see the screenshots below. Clearly this is not a mirror of the original tab. It looks like it is extruding the new tab to the same face the original was extruded to?
How do I mirror just the tab? Attached is the file.
To mirror something it needs to be a separate feature. looking at your screen shots it doesn't look like this is separate but was created with the initial sketch. I can't tell for sure as I am only on 2017. If you will delete the tab from the first sketch and create it as a later feature you will be able to mirror the tab.
Hi Jim! Thanks for your quick reply. The tab is the second feature in the tree (Boss-Extrude2).
Interesting, here is a model using SW 2017. see if it helps, but it looks like just what you did.
Not sure why SolidWorks does not like what you did but you extruded the tab up to surface so when you mirror the tab, it extrudes out to the same surface. To see this for yourself change up to surface to blind.
To fix I would recommend moving the tab extrude above the first mirror. To do this you will need to fix two relations in your tab sketch: Coincident0 and Coincident1 are created from geometry from your first mirror. After you fix the relations, you can move the tab feature above the mirror feature and add it to the mirror feature.
Conrad,
I am only on SW 2015 so I can't open your file, but it looks like one of you settings in your Mirror 2 is not correct since it is looking more like an extrude.
Another thing I think you could do is - do the Boss Extrude 2 BEFORE the Mirror 1 and then you would be mirroring Boss Extrude 1 AND Boss Extrude 2 with the same mirror operation.
For us who do not have your version of SWX it might help if you show an image of just the Boss Extrude 1.
Rick McDonald wrote:
Conrad,
Another thing I think you could do is - do the Boss Extrude 2 BEFORE the Mirror 1 and then you would be mirroring Boss Extrude 1 AND Boss Extrude 2 with the same mirror operation.
Ya, I was on my way out the door and didn't take time to think this though very well. I completely agree that mirroring both features with one mirror would clean things up a little.
Another way would be to split the tab into a separate body and mirror the tab body instead. Of course, this would involve extra steps to split and combine later. I find that this side steps a lot of the errors that mirroring features tend to produce.
It worked fine for me. I suspect that when mirroring you tried to select the tab from the graphics area. Since it was merged with the body when it was created that won't work. It works if you choose the feature from the tree instead.
Thank you all for your help.
Solid Air You are correct it appears Solidworks extrudes the mirror to the original terminating surface. No matter which way you slice it this seems like a bug to me. Notice in the screenshot below the preview appears correct. Do the Solidworks guru's monitor the forum or do I need to report it through official channels?
Solid Air & Rick McDonald You both are correct, I should have mirrored the profile and the tab all in one mirror. This would be the cleaner way to do it and is an acceptable workaround.
Glenn Schroeder I did select the feature out of the feature tree and it still doesn't work. Note I need to mirror about the right plane. Interestingly enough - you found that it does work if you mirror about the front plane.
Thank you all for your help!
-CB
The SW guys do watch the boards and often chime in with advice. However if you find something you would like to see fixed or changed they will tell you on here that you should send it through the proper channels. Open an ER or a SPR through your VAR would be the best way to go. (is there enough alphabet soup there?)
Conrad Buckles wrote:
Glenn Schroeder I did select the feature out of the feature tree and it still doesn't work. Note I need to mirror about the right plane. Interestingly enough - you found that it does work if you mirror about the front plane.
Thank you all for your help!
-CB
I owe you an apology. I didn't pay enough attention to what you were trying to do. I thought you wanted to mirror over the front plane instead of the right plane. To do that you can do as Solid Air suggested, or edit the feature that created that hook, de-selecting the "Merge result" box, then mirror the body instead of the feature, followed by a Combine feature to blend the bodies. See below and attached.
Thank you Glen,
That is another valid workaround. But I believe based on the preview that Solidworks is not behaving as intended.
Also for anyone else interested the same tab geometry gives me errors when trying to make a pattern of it. Based on the screenshots below it seems that mirroring or patterning geometry that was extruded to a specified surface is not acting as it should. These features should pattern and mirror as expected.
As soon as I change the tab from being extruded to a surface to a blind extrude with a set distance everything behaves as normal:
Attached is the file for anyone who is interested.
Conrad,
I'll have to respectfully disagree with your statement: "I believe based on the preview that Solidworks is not behaving as intended". If one feature extrudes up to a surface I'd expect any patterning or mirroring to use the same surface. If you don't want that behavior then it's easy enough to keep the initial feature as a separate body, pattern or mirror the body, and then combine them.
Hi Glenn,
I see your point of view but it wouldn't be a true mirrored feature. In my opinion the feature is fully defined by a sketch surface and by the opposite (extruded to) surface. Now that I have a fully defined feature my opinion is that Solidworks should predictably mirror that feature across any plane and it should retain its form. It should NOT recompute the shape based on the extruded surface.
Maybe it's just my conditioning from years of working with 'other' parametric programs. As with any software I'll need to learn to accept it's quirks I suppose.
Thanks again for your help and advice.
I can also see your point, especially when mirroring.
I wonder, when I made a rapid model yesterday I selected the inside of the leg to create the tab and then extruded up to the outside surface. That might have some effect on why I had no problems
Hi Jim,
I flipped the initial sketch plane to the inside of the leg as you had mentioned, terminated the extrude to the outside surface and now it will not create the feature at all - maybe it's a SW 2018 thing? See screenshot:
That is really strange. Did you open and look at how I did mine? It just fell together, maybe I goofed?
Jim,
Looking at your model I think the difference is you mirrored the entire body. Not saying this is a bad thing but it seems like it's mirroring the main extrusion twice which might have negative ramifications later on in the design.
What I have been trying to do is to mirror just the feature, this is where the problem occurs.
As stated earlier I can include the tab/hook in the original mirror which in most cases is the proper way to model it. BUT the problem is still there when I try to PATTERN the feature. Ironically, which is the way I want to proceed with the design (not mirrored like originally planned).
So my workaround in my current design is to assign a variable to the wall thickness and extrude the feature using that variable. This way if the wall thickness changes, the patterned feature changes, which is the intent of the design.
You all are awesome and I thank you all for your help.
You are right, Ididn't think about that when I did it. That would be another reason for making the tab before the mirror and doing it all with one mirror. I seldom mirror so these are things I don't think about much.
Not sure why SolidWorks does not like what you did but you extruded the tab up to surface so when you mirror the tab, it extrudes out to the same surface. To see this for yourself change up to surface to blind.
To fix I would recommend moving the tab extrude above the first mirror. To do this you will need to fix two relations in your tab sketch: Coincident0 and Coincident1 are created from geometry from your first mirror. After you fix the relations, you can move the tab feature above the mirror feature and add it to the mirror feature.