Revolved Boss/Base


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  1. #1
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    Default Revolved Boss/Base

    Thank you all for the feedback on my last question your replies really help those of us that maynot have your skill sets yet.

    I have encountered an problem with a drawing model I am working on and can't really see what I'm doing wrong, or how to correct it. I attached my part file so you can see what I was up to. The area I can't figure out is when I did a revolve Boss/Base it did this othe cut out as well there should only be the kidney bean shaped hole and not the second hole closer to the nose.

    Any advise would be appreciated concerning what I'm doing wrong and if this is even a good way to approach this part.

    Thanks,

    Dale

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    Default Re: Revolved Boss/Base

    Quote Originally Posted by dkrenfrow View Post
    Thank you all for the feedback on my last question your replies really help those of us that maynot have your skill sets yet.

    I have encountered an problem with a drawing model I am working on and can't really see what I'm doing wrong, or how to correct it. I attached my part file so you can see what I was up to. The area I can't figure out is when I did a revolve Boss/Base it did this othe cut out as well there should only be the kidney bean shaped hole and not the second hole closer to the nose.

    Any advise would be appreciated concerning what I'm doing wrong and if this is even a good way to approach this part.

    Thanks,

    Dale


    Your revolve feature is not a simple revolve, but a revolved thin feature. Thin features are ones where instead of extruding or revolving a selected 2D area, you extrude/revolve a line that has been converted into an area using a thickness offset. You could think of it like extruding/revolving a line into a surface and then adding thickness to that surface to create a solid. In your example the thickness value is large enough that most of the revolved area is filled in, except for that small area. Unfortunately once you create a thin feature you can't convert it back to a normal feature. You have to delete it and recreate it as a non-thin feature. It's not a big deal in your file since you only have one other feature after it, but it can be annoying in a more complicated part.


    As for this being a good way to approach the part, that depends on a lot of things. It mostly just depends on what you want to end up with. It's also a good idea to think about how the part will be made. If it's going to be milled from a solid or cut with some kind of cutting machine (laser, plasma, waterjet) you probably would be better extruding from a 2D sketch. If it's to be 3D printed or molded then it doesn't matter as much. Design for manufacturing is a HUGE topic though so ultimately there are really no wrong answers, just better or worse answers.


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    Default Re: Revolved Boss/Base

    One of my biggest beefs with Solidworks is it LOVES to leave little tiny lines that screw up everything. Take a look at this screen shot. You probably missed it. That's why it has been forced to a thin feature. The other issue is you have no defined sketch. Your axis of revolution is not collinear. Make sure to define your sketches and you will avoid a lot of issues. Revolved Boss/Base-key-cnc-jpg

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    Default Re: Revolved Boss/Base

    Quote Originally Posted by warrenb View Post
    One of my biggest beefs with Solidworks is it LOVES to leave little tiny lines that screw up everything. Take a look at this screen shot. You probably missed it. That's why it has been forced to a thin feature. The other issue is you have no defined sketch. Your axis of revolution is not collinear. Make sure to define your sketches and you will avoid a lot of issues. Revolved Boss/Base-key-cnc-jpg

    I did notice that extra little arc, although when I tried revolving the sketch it didn't start it as a thin feature (which is why I didn't mention it). Now that I try it again I realize that it only starts it as a thin feature if the sketch isn't already being used by another feature. Basically what I did was to roll back the history to before the revolve was created and then create a new revolve, without deleting the old one. So because of that it started as a solid feature and not thin (but did require selection of the closed area). Indeed if you delete the revolve first and then start over with just the sketch, it does automatically turn on thin feature. In that case you can still turn it off though and select a closed area.

    Now here is where it gets weird. I also checked the sketch itself for proper revolve geometry (Tools->sketch_tools->check_sketch_for_feature) and it did NOT flag it as having open and closed contours, meaning that it is (supposedly) ok for revolving. Turns out, not deleting the old revolve first also affects the geometry checker. Because if you do delete the old revolve first and then check the sketch, it says it DOES have open and closed contours (and therefore *should* be fixed first). To me this is a bug! The sketch checker should give you the same results regardless of whether a sketch is being used by a feature or not. It's very strange.

    But anyway, it is better to not have extraneous stuff in your sketches.


    Regarding the under defined sketch; yeah it is better to fully define your sketches. I tend to give people the benefit of the doubt though and not mention it unless it's directly causing a problem.


    The thing about leaving tiny lines behind; I've haven't seen that Solidworks is especially bad in this respect. If you use the trim tool a lot you do have to be careful with what you're doing. But that would apply to any CAD software.


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