Changes to Remote Solve Manager (RSM) at ANSYS R18.0, for Remote Number Crunching

As you may be aware (and even if you did not know!), there are quite a few changes made to RSM at R18.0.

The premise behind these changes is to have RSM provide a simple scheduling tool for customers that don’t need a full-blown cluster installation. This is good for a user environment with a small pool of simulation users. The advantage is that it is straight forward to deploy and use.

When a company starts evolving into using simulation in more facets of design, or when the number of users increases, 3rd party schedulers are suggested for deployment. Examples of 3rd party schedulers are Windows HPC, PBS Pro, and LSF. (For information on supported schedulers and other aspects of ANSYS software, visit this page.) Continue reading

Advertisements

Take Advantage of Repeatedly Used Components in CAD by Instance Meshing in ANSYS Mechanical

Repetitive meshing tasks can be a significant portion of the time a user spends setting up an FEA model for simulation. In cases where components are reused multiple times in an assembly, the meshing can be tedious.

Select 20 of the exact same face in a bolt circle to specify the number of elements on an annulus…

Select the 20 bodies that those 20 faces belong to for a mesh method…

What if the number of bodies/faces/even edges is larger? Continue reading

Restarts in ANSYS Mechanical Can Save Time and Effort!

‘Restarting’ the process in ANSYS Mechanical Products by which a model is solved starting from a previously solved point. The previously solved point contains data for all nodes/elements in the model; there is no results mapping and interpolation when a restart is performed. This is the most accurate method for starting an analysis from a previously solved point.

By default, restarts are not kept when a simulation finishes. The user must modify the Analysis Settings in ANSYS Mechanical to keep the restarts points that will be needed. Those options are shown below:

restart1

Restarts do have limitations. For instance, modification of loads in a step before a restart point is to be used invalidates that restart point. Several tables in the ANSYS Help documentation characterize what happens to restart points if objects in the model tree are changed. This section can be found in Mechanical Applications > Understanding Solving > Solution Restarts, as shown.

restart2

Here’s one of the tables showing where restarts can be used followed by common questions we related to restarts.

restart3

What can solution restarts be used for?
For cases where some subset of the loads does not change and only a few loads change/vary. This is commonly referred to as load case modeling. ANSYS Mechanical FEA can do load case modeling.

Can you give an example of load case modeling?
A model that solves bolt pretension in the first several steps and then locks them in place. Commonly, service loads are applied after the bolt tightening is simulated. The service loads can represent multiple load cases, say one load case is a pressure load, another is a force load.

Another example is a ROPS (Roll Over Protection System) analysis, where loads are sequentially applied on a structure until some criteria is met (usually energy dissipated by the structure). Once the criteria are met for one load case, the load is removed and another load is applied. This process can also be done via restarts.

Why would we do this?
This saves time on solving models. Using the example above, without restarts, the bolt pretension steps would need to be solved every time a load case is added/modified. With restarts, loads can just be activated/deactivated in a step following the bolt pretension and the bolt pretension final step used as the restart point.

Things to know before attempting this method:
All of the load cases that will be solved should be known beforehand. The restart analyses require that ALL loads are defined in the initial model. In ANSYS Mechanical, loads cannot be added to the model tree without invalidating the previous results (ignoring the ability to use restarts).

Newly added loads also will not be applied in a restart analysis as the restart method does not create new elements for these new loads.

If bolt pretension is to be used, any loads defined for a load case should be applied in a step after the final bolt pretension, as usual.

Also, if bolt pretension is used, a step after the final pretension occurs IS REQUIRED. If this is not included, ANSYS assumes the last bolt pretension will be Loaded and not Locked. This means that ANSYS would modify the pretension to maintain whatever preload you have assigned, rather than applying the service loads as a working load on the bolt. Physically, it would be like tightening/loosening the bolt as the service loads are applied.

Method:
The general steps to this method are as follows:

  1. Set up a model with all of the loads applied to the structure. This includes bolt pretensions and any loads that need to be simulated for the load cases. Set up the Analysis Settings as required for the analysis (multiple load steps, Large Deflections, etc.).
  2. Modify the Restart Controls to keep all restart points once the model is solved.
  3. Modify the loads for the load case studies to be inactive.
  4. Solve the model.
  5. Duplicate the analysis, sharing the Engineering Data, Geometry and Model cells. This guarantees the model setup remains the same for all models.
  6. In the new system, activate the load for the first load case study.
  7. Use the Tools > Read Results File… and locate the file.rst from the previously run analysis. This imports the results data into the model.
  8. Modify the Restart Analysis options in Analysis Settings to restart from the end of the first simulation (the final bolt pretension loading, for example).
  9. Solve the model.

Example:
The example shown here uses an oil field fluid end model with bolt pretensions applied. There are two load cases: 1) a pressure load on the cylinder bore, 2) a force load applied on one side of the fluid end body.

Customizing the Output in ANSYS Mechanical with User Defined Results (UDR)

In many situations, we have seen customers ask for ways to output custom results from ANSYS Mechanical. The usual results like Total Deformation, Equivalent Stress or Equivalent Plastic Strain may not be enough for your needs. Depending on the requirements (say a specification you are designing a part to), you can create a User Defined Result to output the needed result. ANSYS already outputs various quantities via User Defined Results that can be viewed in the Worksheet. Here is a quick look at some of what is available:

These quantities are used to create your own results output. User Defined Results can be operated on in several ways. Here is an excerpt from the ANSYS Help documentation (Mechanical Applications > Mechanical User’s Guide > Using Results > User Defined Results > User Defined Results Expressions):

Just as a simple example, say Total Deformation is required and is not output automatically (it is, just an example). If you add an UDR to the results, then type in the expression sqrt(Ux^2+Uy^2+Uz^2), keeping in mind these expressions are case sensitive, you get to resultant deformation from all three component values. Compare this to Total Deformation.

One can also do something more complex, say safety factor calculations. If your specified safety factor is not directly related to the Yield Strength or Ultimate Strength of the material, but some factor of, an UDR can be used; constants can be created and used just like any User Defined Result in the Worksheet. An example is shown here, where a safety factor is calculated based on a value of 6,200 psi. The safety factor looks at the First Principal Stress output, computes the safety factor, then caps the display at 7. Values less than 0 psi (compression when looking at the First Principal Stress) are set to the highest safety factor allowed (7 in this case).

A small note on the equation written in the graphic, in order to display a constant value (0 or 7 in this example), it must be multiplied by the identity matrix (matrix of 1’s). If you are just using a constant for equation manipulation, the identity matrix is not required.

User Defined Results can be a powerful tool if the output from ANSYS Mechanical isn’t quite tailored to your needs.