I'm having problems shelling this model. I keep getting the shown error message. I'm not sure where exactly the problem is coming from.
I'm sure someone here will be able to figure it out.
Thank you . Frank
To start with, one end of the profile in Sketch1 was not tangent, but it was fully defined. This again feeds into the hysteria about fully defining sketches, even if they are wrong.
The shell is doing some really odd things. In this image, it is showing some rolled back features being the cause of the failure.
Next, it's getting the very, very old "Remove Dimension Breaks" bug when a shell fails. I thought this one was documented at least 6 years ago, maybe 10.
Next, it fails if the shell is placed after Revolve1, and a Tools/Check shows that the min radius is somewhere on the loft. But shelling the loft doesn't fail.
The loft is very over constrained. I "fixed" it by adding short lines to the end profiles to make them match the center profile, so it lofts with 3 distinct faces instead of blending the entire feature into a single face. You had a line and an arc on the ends, I put lines on the ends of the arc. I also changed the loft so it doesn't show a flat on the end, it buries itself into the torus. This removes the need to use a fillet to cover the flat end.
Next, the revolves shell out funny because there is no vertical wall on them. The outside donut is 180 degrees, but the inside donut, when shelled, is more than 180 degrees, as you see here:
So I added a small fillet to the outside interior corners.
I don't know how thick you were trying to shell it, but here it is at .75 mm after a lot of messing with it.
The quirks of the shell feature are more than a student should be expected to have to manage.
If you are doing this with sheet metal, it might be better to use sheet metal functionality with forming tools than to try to shell this
Seems like your problem lies on the Revolve1.
R1 has to be increased, I tried 2.00mm and the shell feature works.
So if you gonna put 1.00mm will the machinist able to machine your intention?
Irvin, This is a metal stamping. And just an SW exercise.
Thank you for your help.
Frank... Does this give you a hint on what the problem might be?
If you are going to stamp this your going to need some radius between the features. Probably much larger than I made it.
I'm not going to manufacture this part. I am not a designer. I'm not employed to use SW. I am a student of SW. I am learning SW. This drawing is a SW practice model.
In regards to your response "Failed to find new geometry for existing edge" ?
No, I'm not understanding what your saying. Do I need to remake the file a different way ?
Did you examine the file I attached ?
You are baffling me!.. I will stay out of this (once again)
Now I am baffled.
I thing this is a YouTube video. I have done this before if you correctly follow the video there will not be any issue.
SolidWorks Tutorial # 292: Shelf holder / (2 methods , sheet metal) - YouTube
Yes, I have watched the video and remade the file 2 times. I attempting to discover the mistake is why I'm here. But the fact that the video has been edited in several different spots may not help.
Dennis, though you backed out, you have helped me. I never new you could pin point the problem areas on
a shell like you have shown. I used to just poke and hope till the problem went away. Thanks!
But thanks for your attempt. Have a nice day.
Have you read the warning message?
What this says is while attempting to do the shell, the function failed because the offset caused some of the radiuses/diameters to become null or to cross each other.
I am not much of a surfacer, but I'd use the advices given by SolidWorks. use the Tools check to find the minimum radius required and remove any unintended small faces or edges.
I've read it several times. I just did a search for "Tools Check" (I'm assuming this is some sort of feature or tool ?) but I'm not finding it any where. Can you show me where I would find this "Tools Check" ?
No problem buddy, it can be confusing, it's actually the check tool which is located in the Tools menu.
Using the Check Tool for Minimum Radius of Curvature
2016 SOLIDWORKS Help - Check Entity
When you create a shell, SW offsets the faces and features that are being shelled. When you offset a fillet, which is an inside corner, the radius grows, due to the offset. When you offset a radius, which is an outside corner, the radius shrinks, again due to the offset. If your radius is smaller than the shell thickness, the radius becomes negative, so the shell fails.
Your cut aways got me thinking. As it turns out I missed some 1 mm fillets at the base of the loft and around the eyelets. When Dennis Bacon sent me the screen shot at the beginning of this tread of the error flags, I could not make out the point of where they where coming from. It was too blury. Once I was able to figure out how to replicate and then study his sceenshot, between his and your responses, I figured the shell out.
Thank you for your time and effort.
Thank you all !
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