someone please help me figure out why this is happening. The edges of the loft seem to be connecting but it leaves the inside completely hollow, resulting in zero thickness geometry error.
Thanks in advace
Hello Ryan,.. first check if you have VOR on or off? (Tools/Options/Verification On Rebuild)
..if it creates that error both on/off... you may have to slightly move/offset the sketch inside the volume.
I checked and it does the same thing with the VOR on and off. I attempted to move the sketch back into the volume but it doesn't seem to do anything. I will have to check to see if I am moving it far enough inside and let you know.
Hello Ryan,.. I can see the file and see what is going on... yeah, you have have few issues here.. and mixing a 3DSketch onto a Surface/Solid.. is lowering the accuracy... it is NOT a good combination... (do not use the 3DSketch7, imho)
So.. the other recommendations of offsetting the split surface area on cylinder (again, do not use the 3DSketch7)... but lofting or using Boundary(better)) between faces would be better.. (image/file (2017) attached)
Attach your file pal....
Here is the part file if can help me create this loft I would greatly appreciate it.
It is a bit of a "brute force" workaround, but you can make it work by creating boundary surfaces of the two 3DSketches and then creating the loft.
I know there should be a cleaner way to accomplish this, but I don't really have much time to play around with it.
I appreciate your effort and really wish I could open the part but unfortunately I am running SW 2017 sp3. I am completely fine with workarounds at this point. I have spent far too much time attempting to solve this problem. I'll try making the boundary surfaces myself and attempt the loft. Thank you!
OK I will show you step by step be patience...
It worked provided that both of these boxes are unchecked. I can understand 1st box. I do not know why 2nd box?
I think there's a error of 0 thinchness ... did you see my part? one has 1mm of interference on the another
I was unable to open the part since I'm running SW 2017 sp3. I am attempting to follow your step by step solution but I am getting a 0 thickness error. Thank you for all of your help thus far, it is much appreciated.
I send you the video maybe it will be usefull to you....be patience pal...every path go to Rome....
Fix - YouTube
Thank you! I will check it out. I definitely learned a few things from your method.
To expand on Maha's solution,
Create the loft but uncheck the merge option so that there are two separate bodies in the model.
Offset the inner face of the lofted body so that it's inside the outer wall of the first body.
Combine the two bodies.
The net result is essentially the same solution that Paul Salvador suggested only without offsetting the inside geometry.
The quickest solution that I have found is to make a Filled Surface with 3DSketch1, and then loft between Split Line1 and the newly created surface. You really don't need 3DSketch7 if you use this technique.
Whenever of one part interferes with the other, any way would be fine. The problem is always the thickness 0 in some contact area
I finally figured it out.....well, I got it to work, not exactly sure why this solution worked for me and not the others. I created a filled surface with 3DSketch1 and then lofted (merge result) from that surface body to 3DSketch7 with a guide curves connecting each of the bottom corners. Thank you to everyone for all of your help, I greatly appreciate it!
You won't even need to add guide curves if you go from the Split Line1 to the new filled surface.
(see my most recent post.)
What is different between filled surface and off set surface (I mean 0 thickness) for a sketch that is already on surface. Because I found that in both cases sketch behaves differently.
Maha Nadarasa wrote:
I'm not sure what the difference is between the way SOLIDWORKS handles the two different types of surfaces.
When I initially made filled surfaces for both of the 3DSketches, I thought I saw a difference between the filled surface and the Split Surface (I did not try the 0 offset surface.)
There were definitely some interesting things happening with this model.
By using the Split Surface, you won't even need the 3DSketch that is on the surface or the 0 offset surface.
Thank you, I appreciate all your help oddly enough I was unable to select the Split Line1 for the loft. Again, not sure why but glad we collectively found a workaround
Retrieving data ...