## General Mechanical

#### Ansys workbench

• Ayman
Subscriber

how can i apply these steps:

1-In the first step, the beams were simply supported at both ends. The column and the blind bolts were fixed temporarily in case of the motion of free bodies. Meanwhile, a low level of pretension was applied to all bolts to ensure that the contact interaction had been established.

2-In the second step, the temporary constraints for the column and blind bolts were removed, and the bolt pretension was increased to the value that was mentioned above. Simultaneously, the vertical loading was applied on top of the column through displacement control up to 110 mm.

• peteroznewman
Subscriber

I recommend you simplify the model. Since the geometry and loading appear to be symmetric, you could slice the model in half with a YZ plane through the center of the tube using the Symmetry function in DesignModeler.  Then you can slice the model in half again on the XZ plane.  If you aren't using DesignModeler, you can cut the solids using those planes in any CAD system and apply Symmetry boundary conditions in Mechanical.

Insert a Contact Tool under the Connections folder and ensure that all the contacts are closed. That means bolt heads and the flange against the center tube. If a contact has a very small gap, use Adjust to Touch to close the contact.

Under Analysis Settings, set Number of Steps to 2 and make sure that Large Deflection is On.

Add a Remote Displacement to the top face of the center tube. The constraint is Z = -110. Look in the Tabular Data window. Set step 1 to have Z = 0, and step 2 to have -110. If you are not using YZ symmetry, you also need X = 0 for steps 1 and 2.

To get a roller support on the ends of the side arms, create a Remote Displacement 2 at the end face of a side arm. If you did not use symmetry, add a second Remote Displacement 3 at the other end face of the other side arm. The constraint can be  Z = 0 if you used XZ symmetry. If you did not use XY symmetry, then you also add Y = 0 and Rot X = 0 to Remote Displacement 2 and 3.

Step 1 should only have the Bolt Pretension coming to the full value.

Step 2 has the change in the Z value of the Remote Displacement.

• Ayman
Subscriber

@peteroznewman thank you for replying to my question can you explain more about contact tool that make contact closed iam aleardy create a friction contact between bolt heads and the flange with 0.1 coefficient with no gap between them and bonded contact between bolt and nut.

about the first step the bolt pretension coming to the full value (60000 N) and second step the bolt pretension stay at this value  (60000 N) or come to zero.

• Ayman
Subscriber

@peteroznewman after I applying your steps for boundary condition and check the contact using the contact tool I get the following error:

1-Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully.

2-One or more objects is using a deformable behavior but is applied to a collinear set of nodes.  This is not recommended and can cause solver difficulties.  Check the Solver Output on the Solution Information object to identify the offending load.

4-An error occurred inside the SOLVER module: general error.

then the model fail.

• peteroznewman
Subscriber

1- is a warning, not an error.

2- is a warning, not an error.

3- Did this happen on the first substep?  If so, insert a Contact Tool under the Connections folder and Generate Initial Contact Status. Open that to look to see that all the contacts are closed. Reply with an image of that table.

4- Solve problem 3 first.

• Ayman
Subscriber

Yes it happens on first substep

• peteroznewman
Subscriber

Maybe warning #2 is the source of the problem.  Things are a lot easier if you make two slices and use 1/4 symmetry. That immediately takes away 5 DOF, therefore, as long as you constrain just one point in Y, you might resolve this error.

Next time you have a Contact Table, click on the Status column heading and group all the inactive rows together, you don't need to show those and it will cut your screen grabs in half.

• Ayman
Subscriber

@peteroznewman can you check my model file because my doctor wants to solve the whole model first the simplify it and compare them then make changes to the model and apply the parametric design.

• Ayman
Subscriber

@peteroznewman sorry for disturb you again I study this model from research attached after I check his practical result I will start my changes to the connection with different boundary condition for my master thesis

but I don't have much time I should finish before 29/08/2020.

• peteroznewman
Subscriber

1) Remesh the flange and put at least 2 elements through the thickness. Never have a flat plate in bending with a single layer of solid elements.

At some point you might need 4-8 elements through the thickness.

2) You need to turn on Automatic Time Stepping for Step 1 and have 10 Initial Substeps.

3) Go back to CAD and use Divide Face to split the cylindrical face on each of the bolts at the nut boundary.

If you add two planes of symmetry, you would only have to do 4 bolts instead of 16 bolts.

4) Delete the Remote Displacement at the center and create one that only pulls on the bottom face of the center tube. You currently have it scoped to 3 faces. Don't do that.

• Ayman
Subscriber

@peteroznewman  i follow your steps and create two symmetry plans but I still have the same error:

• peteroznewman
Subscriber

You split the face of the fastener, but you didn't move the Bolt Pretension to the face between the head and the nut.

The image on the left has the Bolt Pretension on the face that is bonded to the nut.  Wrong.

The image on the right is the correct fact to use Bolt Pretension on.

You didn't change Step 1 to Auto Time Stepping with 100 Initial Substeps. Change the Solver Type to Direct.

I suppressed the body at the tip of the arm, past the Pin1. It is not necessary.

Under the Solution Information folder, it is best to have non-zero values, like 3, for Newton-Raphson Residuals and Identify Element Violations. They create useful troubleshooting data if the solution doesn't converge.

It is faster to do troubleshooting on just one bolt, since that is where the problem seems to be. Suppress all bodies except these four.

When you solve, you will find the END PLATE 1 is what blows up. If you change that part material back to Structural Steel, you will find this small model converges.

The conclusion is there is something wrong with the end plate material.

The problem is that the units were set to Pa while the numbers you are using are in MPa so you are off by one million.

You have the same problem in all your materials except for Column Structural Steel. That has the proper number to match the units.