Learning Forum

[2851641m]

Got a simple box with composites sandwich panels.

Boundary conditions, fixed at 6 points at the base and then a 16,000N force is applied to the rest of the whole system.

Had issues trying to solve with direct solver but error "This model has a remote point with one or more constraint equations that has more than 40000 terms. This will lead to significantly higher memory requirements and solution times. The solution is terminated, refer to output file for more information."

So switched to an iterative solver which fixed it but is confusing cause now not getting a force convergence plot so can't check if it has convergaed correctly.

1. How could I overide the may lead to high memory requirments and just let it run for ages so can use a more acctuate direct solver
2. Why can't I see the force convergance plot and is using an iterative solver valid?

Any help would be very much appricetied!

[peteroznewman]

Don't use a Remote Force to apply load to the entire model.  Please describe the actual physical effect that causes load to be carried by the structure. I see the arrow is pointing sideways.  Maybe you could use an acceleration to represent the force.  What is the mass of the structure?  Calculate the acceleration from F = ma.

If the arrow was pointing down, I would have thought the force was caused by the weight of some fluid in the box. In that case, you could use Hydrostatic Pressure on the faces of the interior of the box.

[2851641m]

Hi thank you for your quick responce, the physical affect is the box is loaded 40g to the side, the box has other stuff in it so will be a greater mass than the model.

I've tried using acceration instead with f=ma, f = 9.81*40*60 m= 30kg a= 785m/s^2.

I get a very high factor of safety which is suprising and no displacement solution. so don't know whats happened.

[peteroznewman]

Use Distributed Mass to add the mass of all the stuff inside the box to the 5 faces of the box as a rough approximation. You need the correct total mass of the box plus the contents to be in the model.

The acceleration to enter in Ansys for a 60g load is 60*9.81 = 392.4 m/s^2.

Please show which faces have the fixed support.

You did not retrieve the Total Deformation from the results file, it has the lightning bolt showing.

Once you get that working, we can talk about a better approximation of the contents of the box.

[2851641m]

Sorry I should have said when I pressed retrieve for the displacement this error ocurred "You have specified result time(or frequency) = 4 for a result file which has maximum time(or frequency) = 1.  If you specify 0(ZERO), the solution for final time will be displayed."

These are the faces with fixed support

[peteroznewman]

Follow the advice in the message and type a 0 where there is a 4 and you will get a deformation result next time you try to retrieve the results.

[2851641m]

Thank you I've fixed that now. But the reserve factor still seams way to low aswell as the deflection

[peteroznewman]

Did you add the Distributed Mass to the box?  Which faces did you select?

To gain confidence that you are using the software correctly, build a simple verification model of the bending of a beam.  Apply a fixed support at one end and apply a moment to the other end. Use beam equations to do a hand calculation for what the deflection and stress should be. This will be simpler to do if you make the composite stackup use only unidirectional plies at 0 angle along the length of the beam. Plot the deflection and stress in the model and check that you get the expected result.

[2851641m]

Got it sorted, it was in mm/^2 so was very very slow accerlation changed it up to m/^2 so all in the ranges I expected.

Thank you for your help!