Can't figure out why the "ribs" (had to loft them cause I couldn't figure out why the rib feature wouldn't work) won't mirror over the Right Plane...
I think minor geometry issues may be the reason for error
Loft1 and Boss-Extrude3 has gap in between
Try Loft1 as a solid body(disable merge option)
Circular pattern body option
Now use combine and add all together to form a single solid
Hope this works
It appears the mirror fails because of the loft feature. If I try to mirror just the loft, the message returned is "Loft operation failed to complete". Also when you are working with non planer surfaces, you run the risk of zero thickness geometry. When I try to extrude your sketch9, that is the message that comes back. That may be affecting the rib feature (I have never used this feature so it is only a guess).
Ben,..agree, with John George and Solid Air.... and I can guess/assume now why you did the Loft.... that is, Sketch12 (the parent of 13 and 14) could have been extruded mid... but it results in a "ztg" (image attached and error)... but your loft (with 13 and 14) it did not give you this error... well.. it eventually shows up later.
Alternate solution for you (since I do not know your design intent). Get rid of the loft (I do not think it gave you the profile for the rib you wanted anyway - curved rib surface). Extend Sketch12 so it goes past the 17.5 diameter inner hub (I used 0.5mm see screen shot below). Now do a midplane extrude to the thickness you want. I still could get the mirror to work after the circular pattern so I reversed the order to get it to work (see other screen shot). So is this for a school project (I see the little graduation cap by the root feature which normally means the model was created in an educational version)?
Thank you all for your help! And, yes, I am back in school, again... I realized a much better solution was to "revolve cut" the contour of the rib then to "extrude cut" out one segment, then linear pattern the cut. Thank you again for taking your time to help me solve the issue.
If that is the design intent of the rib then that is the way to go.
You have two basic issues causing the problem, but they're easily fixed. Edit your Loft, deselecting the "Merge result" option. By doing this the Loft will be created as a distinct, separate body.
Next, edit the Circular Pattern. Clear the selections for "Features to Pattern", select "Bodies to Pattern" instead, and choose the Loft.
Delete the existing Mirror and create a new one, this time selecting "Bodies to Mirror" instead of the default "Features to Mirror".
After doing this you can use the Combine feature to merge the bodies, if needed.
Thank you Glen for taking the time to show me how to fix the issue! As I previously stated, I made it work a different way after getting frustrated, BUT, I really do appreciate you showing me how I could have done it successfully using my initial method. Coming from a MAYA and MAX modeling and animation background, the transition to Solidworks has been a bit tricky and difficult at times. BUT, again I really do appreciate all of the fantastic feedback from everyone. This is definitely one of the best Forums I've ever been in.
Phuc Nguyen, I don't know what format you want me to save it as... It's not possible to save as an "older version" to my knowledge, but I did save it as a .3dxml file... Not sure if that is helpful, but if there's a different format you'd like then please let me know.
Patterns and Mirrors defaulting to Features, and default merging bodies, are two things that cause problems for quite a few people until they learn to watch out for them. I'm glad I could help.
Could you post sldprt in older version so that everybody can follow your query? I've used SW 2016.
Ben,.. Parasolid or x_t or x_b are the native formats for SolidWorks.
I'll attached the original in x_t and/also how I'd model this... but, I think what you did above is very good!
Thank you for letting me know Paul! I'll just upload Parasolids from now on! I liked the simplified steps you took over my final model. Again I can't thank you all enough for the awesome responses and the insights into how to bring my concepts to reality in solidworks!
Good job Paul ! You make everything simple
Appreciate for your help. I've got a notification like that:
Delete Guide Curve #1 for initial method and it works fine in SW2017.
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