You want to reduce your model to the minimum that is required to get some useful information. You have geometry for the handle that is attached to the tube, and you are holding that handle fixed.
Suppress the Handle body and move the Fixed Support to the end of the tube that was fixed to the handle.
The tube is pushing against a flat wall solid body that is much, much stiffer than the tube. Change the flat wall from Flexible to Rigid and the solver doesn't have to calculate the practically zero deformation in the wall.
The next change you need is to put at least 4 elements through the tube wall thickness. You have two or three.
I made the length of the elements a bit longer than I wanted, but this was just to get a first result. See that the rigid surface only has surface elements.
That mesh was able to solve to 60% of the full load before failing.
This took only 111 seconds to solve on 8 cores.
Here is the deformation at 60% load. I didn't check how far you got with your initial model.
I got the same error message you did.
Here are the elements that are failing. They are at the Remote Displacement end.
The corrective action to get the model to make more progress to the full load is to use smaller elements near the end.
There may be an advantage to change the Behavior of the Remote Displacement from Deformable to Rigid, but maybe not. Have to run it both ways to see which one goes further. With those two changes, it got to 76% of the load.
The problem now is just force equilibrium convergence. This solution took 1009 seconds on 8 cores.
There are no more element errors. The next step might be to switch from Static Structural to a dynamics solver since finding equilibruim states from this point forward is going to be very difficult. What speed it the end moving?
Another change that might help down the road is to change from a linear elastic isotropic material to a hyperelastic material.