2D Axisymmetric Cylinder
Hi Justin, welcome to the forum.
You didn't mention what specifically was not working, so here is a list of things that I noticed. Hopefully, one of them will be the solution. 
Of course, all of the drawing-related tasks can be done to the original AutoCAD drawing or to the sketches after you import it.
- The model needs to be positioned so that the centerline is at Y=0.
- The Y coordinate becomes the radius. So, you only need the portion of the model on the +Y side of the axis.
- Each enclosed region needs to be on a separate part. So the 5 welds need to be 5 different parts. If I counted properly, it looks as if you need to have 10 parts in the final model. (See the attached image).
- Each part must be a completely enclosed region. It looks like most of the parts are fully enclosed except for some of the welds. (Once you get it in Simulation Mechanical, you can right-click on a part and choose "Isolate". This will help to show whether the outline is complete or not.)
- If you want the mesh to match between the parts (so that the parts are connected together), the outlines where the different parts match must be the same length. So the side of the tube (part (4) in my figure) should be split or intersected where each of the welds (parts (5), (7), (8), and (10)) meet up.
- To mesh the entire model, right-click on "Plane 2" in the browser (tree) and choose "Select all sketches". You can then generate the mesh using "Mesh > Mesh > Generate 2D Mesh".
- Under the Element Definition for each part, set the "Geometry Type" to Axisymmetric.
If you still need help, maybe create an archive of the model and attach it. See "Create, Post, or Provide an Archive of your model".
______________________________________________________________
If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!
Great! As I told someone else recently, getting results is the first step to getting results
Here are a number of things to investigate about your model:
- Is the constraint on the ring (part 5) correct? The high stress in the welds (parts 6 & 7) may be due to the fact that the ring is fixed from moving. What is holding the ring in place in the real assembly? (See the attached "check constraint.png") Does the real constraint
- There may still be an issue with the shape of the elements. I noticed a very small gap between the ring and tube (part 4 & 3, for example). This leaves a small edge that for an element in the weld. (See the attached "eliminate small gap.png". Sorry, I should have captured an image of the same ring and welds, but I did not
.) I am hoping that the elements will not be so long and skinny by eliminating the gap, and that may improve the stresses. Be sure to set the contact between the ring and tube as "Free/No Contact" so that they are not bonded together. (Select the two parts, right-click > Contact > Free/No Contact.) I think this situation of the small gap appears in 3 locations in the model. - The key question is what happens in real life compared to the analysis. Analysis (FEA) is generally not very good at sharp corners. It acts like a stress concentration -- like a fillet of 0 radius. If this is what is occurring, then the stress will continue to rise as you make the mesh smaller. If the stress calculation is "real", then the stress will stop increasing once you make the mesh "fine enough". So if the problem is the sharp corner, you may need to ignore the result at those spots, and extrapolate the result for the adjacent nodes to get a better estimate of what happens right at the corner. Experience with the real assembly can help here, especially if you can analyze an existing design that you know is satisfactory. If that analysis gives the same high stress, you have some justification to ignore it.
Here are two other thoughts related to the welds, which are not intended to imply that the results can be ignored just because they are high. If other readers have some feedback, please provide your insight. But what I wanted to say is:
- The real situation in a weld is highly complex because of the heat applied during welding. All of the residual stresses that occur are being ignored. (Don't worry, the residual stresses are ignored in 99.95% of analyses.) The stresses being calculated are added to the residual stress, so I do not know if a calculated stress of 80% of yield is acceptable or if the residual stress is so high that a calculated stress of 5% of yield is too high!
- This is just a guess, but I think a lot of things yield in real life. It might be just a spot at a stress concentration, but such yielding "relieves" the high stress, and the load gets distributed to the rest of the assembly. Of course, if fatigue is a concern, then localized yielding can still be a concern. But if a part is basically static, then a small amount of yielding may be permissible.
