ANSYS How To: Result Legend Customization and Reuse

ansys-mechanical-custom-legend-0A user was asking how to modify the result legend in ANSYS Mechanical R17 so Ted Harris put together this little How To in PowerPoint:

padt_mechanical_custom_legend_r17.pdf

It shows how to modify the legend to get just what you want, how to save the settings to a file, and then how to use those seettings again on a different model.  Very simple and Powerful.

ansys-mechanical-custom-legend-1

 

 

ansys-mechanical-custom-legend-2

NICE Desktop Cloud Visualization

nice-dcv-banner

In a previous post I argued that engineers do magic (read it here). And to help them do their magic better PADT Inc. introduced CoresOnDemand.com.

af-1
Among the magical skills engineers use in their daily awesomeness is their ability to bend the time fabric of the universe and perform tasks in almost impossible deadlines. It’s as if engineers work long hours and even work from home, while commuting and even at the coffee shop. Wait, is that what they actually do?

Among a myriad of tools that facilitate remote access and desktop redirection available, one stands out with distinction. NICE-Software developed a tool called Desktop Cloud Visualization (DCV for short). DCV has numerous advantages that we will get into shortly. The videos below give a general idea of what can be achieved with NICE-DCV.

Here is a video from the people at NICE:

And here is one of two PADT Employees using an iPhone to check their CFD results:

Advantages of Nice-DCV

Physical location of cluster/workstation or the engineers becomes irrelevant

Because engineers have fast, efficient and secure access to their workstations and clusters, they no longer need to be in the same office or on the same network segment to utilize the available compute resources. They can utilize NICE-DCV to create a fast, efficient and encrypted connection to their resources to submit, monitor and process results. The DCV clients are supported on Windows, Linux & IOS and even have a stand-alone Windows client that can be run on shared or public computers. In a recent live test, one of our engineers was travelling on a shuttle bus to a tiny ski town in Colorado, he was able to connect over the courtesy Wifi, check the status of his jobs and visualize some of the results.

af-2

The need for a powerful laptop or remote workstation to enable offsite work is no longer the only solution

There is no need for offsite engineers lug around a giant laptop in order to efficiently launch and modify their designs or perform simulation runs. Users launch the DCV client, connect to their workstation or cluster and are immediately given access to their desktop. No need to copy files, borrow licenses or transfer data. Engineers don’t need to create copies of files and carry them around on the laptops or on external storage which is an unnecessary security risk.

af-3a

 “If it ain’t broken don’t fix it!”

Every engineer uses ANSYS in his own special way. Some prefer the good old command line for everything even when a flashy GUI option is available. Others are comfortable using the Windows like GUI interface and would

af-3

Opens the door for GUI-only users to utilize large cluster resources without a steep learning curve or specialized tools.

Nice-DCV makes the use of ANSYS on large HPC clusters within reach for everyone. Engineers can log into pre-configured environments with all of the variables needed for parallel ANSYS runs already defined. Users can use can have their favorite ANSYS software added to the desktop as shortcuts or system admins can write small scripts or programs that serve as an answer file for custom job scripts.

From 0-60 in about…10 Minutes

For an engineer with the smallest amount of system administration skills it takes about 10 minutes to install the Nice-DCV server and launch the first connection. It’s surprisingly simple and straightforward on both the server and the client side. The benefits of Nice-DCV can be immediately realized in both simplified cluster administration and peace of mind for both the engineers and the system admins.

PADT’s CoresOnDemand and Nice-DCV

The CoresOnDemand service that PADT introduced last year utilizes the Nice-DCV tool to simplify and enhance the user experience. If you are interested in a live demo on Nice-DCV or the CoresOnDemand environment contact us either by phone: 480-813-4884 or by email cod@padtinc.com. For more information please visit: CoresOnCemand.com

(Note: some of the social media posts had a typo in the title, that was my fault (Eric) not Ahmed’s…)

Using Probes to Obtain Contact Forces in ANSYS Mechanical

Recently we have had a few questions on obtaining contact results in ANSYS Mechanical. A lot of contact results can be accessed using the Contact Tool, but to obtain contact forces we use Probes. Since not everyone is familiar with how it’s done, we’ll explain the basics here.

Below is a screen shot of a Mechanical model involving two parts. One part has a load that causes it to be deflected into the other part.

p1

We are interested in obtaining the total force that is being transmitted across the contact elements as the analysis progresses. Fortunately this is easy to do using Probes in Mechanical.

The first thing we do is click on the Solution branch in the tree so we can see the Probes button in the context toolbar. We then click on the Probe drop down button and select Force Reaction, as shown here:

p2

Next, we click on the resulting Force Reaction result item under the Solution branch to continue with the configuration. We first change the Location Method from Boundary Condition to Contact Region:

p3

We then specify the desired contact region for the force calculation from the Contact Region dropdown:

p4

Note that the coordinate system for force calculation can either be Cartesian or Cylindrical. You can setup a coordinate system wherever you need it, selectable via the Orientation dropdown.

There is also an Extraction dropdown with various options for using the contact elements themselves, the elements underlying the contact elements, or the elements underlying the target elements (target elements themselves have no reaction forces or other results calculated). Care must be taken when using underlying elements to make sure we’re not also calculating forces from other contact regions that are part of the same elements, or from applied loads or constraints. In most cases you will want to use either Contact (Underlying Element) or Target (Underlying Element). If contact is non-symmetric, only one of these will have non zero values.

In this case, the setting Contact (Contact Element) was a choice that gave us appropriate results, based on our contact behavior method of Asymmetric:

p5

Here are the details including the contact force results:

p6

This is a close up of the force vs. ‘time’ graphs and table (this was a static structural analysis with a varying pressure load):

p7
p8


***** SUMMATION OF TOTAL FORCES AND MOMENTS IN THE GLOBAL COORDINATE SYSTEM *****

FX = -0.4640219E-04
FY = -251.1265
FZ = -0.1995618E-06
MX = 62.78195
MY = -0.1096794E-04
MZ = -688.9742
SUMMATION POINT= 0.0000 0.0000 0.0000

We hope this information is useful to you in being able to quickly and easily obtain your contact forces.

Making Charts and Tables in ANSYS Mechanical

imageOne of the nicer features in ANSYS Mechanical is the fact that when you enter in any type of tabular data, or look at any type of tabular results, you can view it as a table or as a graph.  But what if you want to make your own graph, maybe even viewing values from two different solutions?  ANSYS Mechanical has a little used feature called “New Chart and Table” that will allow you to make a table or a graph (chart) of quantities in your model tree that make sense when displayed as a graph or table: Time, loads applied over time, and results over time.

image

I have found myself exporting data to excel and making graphs all the time. And this is OK if you just do it once. But if you make a change to the model, you need to export again and redo your graph.  The Chart and Table function makes this an automatic step, right there in your model tree.

For this posting, we will just use a simple plasticity bending example. We hold the bottom of a round bar with a grove cut in the bottom part and push on the top with forces.

In its simplest form the “Chart and Table” duplicates what you see in the graph and Tabular Data windows when you click on a load or a result. Here is what you get when you click on a displacement:

image

And if you select the probe in the tree and click on the “New Chart and Table” icon you get:

image

No woop.  But even if I want to just plot one value, I can now customize the look of the graph a bit.  Take a look at the Details for the Chart:

image

With the Chart Controls you can define what is shown on the X axis; if you want lines, points or both with Plot Style, log or linear scale, and if you want horizontal, vertical, neither, or both gridlines.

image

This is what it looks like if I turn on both gridlines and use a log scale for the Y Axis.

Next, we can add axis labels with “Axis Labels:”

image

The “Report” Section tells the program what to do when a report is generated. By Default you get a table and a graph.  But you can do either, both, or you can suppress it in the report.  You can give the plot and/or table in the report a caption by filling in the Caption field.  It comes out nice:

image

Note that it actually includes a legend in the report. If you want the legend when you are looking at a graph interacively, just Right Mouse Button on the graph and choose “Show Legend” to turn it on:

image

image

Note that the legend shows the name of the branch in the tree. That is not very informative. So I change it to something useful and now the legend is useful:

image

 

So even with a basic graph, we can do a lot. But the real power is when you want to look at more. Let’s say I want to plot the force and the stress over time. I create a new chart with the icon then select the force and the stress results as my “Outline Selection”

image

I get a lot of stuff on my graph. That is because the program starts by plotting all the components for the load, and all max and min stress over time for the result. I simply change the ones I don’t want from “Display” to “Omit.”  Then I get:

image

Much more useful.  Note that it does not create two separate Y axis. Instead it normalizes the values between the min and max for each. This is not ideal, and hopefully in the future they will support multiple axis, but it still works for most cases when you want to compare things. Note that I renamed the branches in my tree so they show up in the legend correctly.  Next I will add some labels and turn on gridlines.

image

We have been neglecting the table. It also gets created:

image

As with any table in ANSYS Mechanical, it can be exported to Excel. So if you find yourself grabbing data from multiple input or result tables and pasted them into Excel, make a Chart and Table item to grab all the data you want in one place, then export it once.  To be honest, the quality of the graphs that are made are good enough for engineering, but maybe not good enough for a presentation. By making a Chart & Table of what you need, then exporting to Excel or some other graphing tool, you can still save a lot of time.

Next, let us look at plotting values from multiple simulations.  If you look at the tree, you will notice that the charts are a child of the model, not the simulations.  This signals that we can show data form the same model, but different simulations:

image

In our example I’ve simply made one with a tip force in the Y direction, and one with a tip force in the X direction. And I can show that by making a chart:

image

And I get a table:

image

HINT: If you want to make a single table or chart that shows all your input loads over time, in a single simulation or across multiple simulations, this is the way to do it.  If I add a third simulation where I vary the load in all three directions, I can capture all three cases in one table:

image

These examples show loads. Here is what it looks like if we review the deflection on the tip probe over time for two simulations:

image

Or mash it all up, and show stress and deflection for both cases:

image

In every case so far we have used time (Load Step for static) as our X axis. But you can put any value you want on the X axis.  Here is Force applied vs Tip Deflection:

image

Make sure you turn off Time and loads you don’t want to see.  This is a great way to plot hysteresis effects.

You may notice the plots in this posting are nice and big and have a good aspect ratio. And your screen looks like this:

image

Every window in ANSYS Mechanical can be dragged out of the frame and positioned/sized however you want. So I pull off the Graph window by itself and resize it to the aspect ratio I want. Now when I want to save the image all I have to do is select that window and hit Alt-Print Screen. The image is now stored in the clipboard and I can past it where I want.

image

To get the normal window configuration back, click View>Windows>Reset Layout.

As always, play with it to figure more out. I’ve included my simple test case in case you want to play with it first:

Utilizing a Thermal Contact Conductance Table in ANSYS Mechanical

We recently had a tech support request from a customer, asking for the ability to define a spatially varying thermal contact conductance (TCC) on a contact region in ANSYS Mechanical. We came up with a solution for ANSYS 14.5 via an example which includes a couple of verification plots.

The test model consists of two solids, connected via a contact region. The thermal contact conductance at the contact region was defined as a table, with the rows and columns of the table corresponding to local coordinates within the plane of the contact surface. The table was defined and implemented using Mechanical APDL commands in the Mechanical tree.

Low values of TCC were used for testing purposes. This helped verify that the tabular values were actually being used as intended. A constant temperature was applied to the face at one end of the model, while a different constant temperature was applied to the face at the extreme other end of the model. This temperature differential caused heat to flow through the contact region, subject to the resistance defined via TCC values.

The coordinates in the plane of the contact surface were Y and Z. Thus, the table of TCC values varied in the Y and Z directions, as shown here:

            Z        
  Y |  0.0        1.0
0.0 | 0.0001    0.0005
1.0 | 0.0005    0.0002

Three ANSYS Mechanical APDL command objects were inserted into the tree in the Mechanical editor. The first command object simply added a scalar parameter to keep track of the contact element type/real constant set number for use later:

The second command object was placed in the analysis type branch, meaning this set of commands would be executed just prior to the Solve command. This command object does three things:

1. Defines the TCC table vs. Y and Z coordinates.

2. Reads the table in as an MAPDL real constant for the contact elements identified in the first command object.

3. Issues the command, “rstsuppress,none”. More on this later.

This is how the second command object was defined:

That third step mentioned above was a key to getting this technique to work in 14.5. The rstsuppress command is not documented currently, but Al Hanq of ANSYS, Inc. has told me that it will be documented in the future. The default setting turns off contact results from being written to the results file in a thermal analysis. The idea is to help keep results file sizes from getting excessively large, especially for transient thermal runs. In this case, we actually wanted the thermal contact results in the results file, so we issued “rstsuppress,none” so the thermal contact results were not suppressed.

The final command object was for verification of the applied TCC values. This set of commands generates two plots using MAPDL postprocessing commands. The first plot is of heat flux going through the contact elements. The second plot displays the TCC values for node ‘i’ of each contact element (averaged).

Here is the third command object:

Both of these plots show up in the tree, labeled as Post Output and Post Output 2 in the image above.

This is the resulting thermal flux at the contact surface:

Here is the applied thermal contact conductance, as mapped from the table defined in the second command object:

In summary, we took advantage of Mechanical APDL command objects to apply thermal contact conductance values that vary along the contact region. We also used MAPDL commands to create two plots that help verify that the TCC values were applied as intended. Hopefully this is a helpful example.

Saving Mechanical APDL Plots in a Design Study

One of the cool features in the ANSYS Workbench is the ability to set up a design study and kick off a bunch of runs that bring back key parameters.  This is great for a design exploration but sometimes you actually would like a result plot, or maybe the info in a text file as well.  When a design study is done, unless you tell Workbench to save all your run files, it deletes all the files.

To do the posting on ICEM CFD in the workbench project page, I needed to do just that, so I thought I would share my method in case others want to use it.

The way I do it is pretty simple:

  • Use a /INQUIRE to get the directory the run is running in
  • Use some string functions to get the name of the design point from the directory name
  • Temporarily change the jobname
  • Save my plots
  • Change the jobname back to file
  • Copy the files to the User_Files directory.

Here is what it looks like:

   1: /post1

   2: set,last

   3: finish

   4: /inquire,aa,directory

   5: ii = strpos(aa(1),'\dp')

   6: ij = strpos(aa(ii+1),'\')-1

   7: dpn = strsub(aa(1),ii+1,ij)

   8: dpn = strcat(dpn,'_')

   9: /file,dpn

  10: /post1

  11: /view,1,1,1,1

  12: /vup,1,z

  13: /show,png

  14: eplot

  15: plnsol,u,sum

  16: /show,close

  17: /sys,copy *.png ..\..\..\user_files

  18: finish

  19: /file,file

See how it uses /inquire to get the directory, then strpos(), strsub(), and strcat() to get the design point name.  Then it simply changes the file name, does a /show,png and plots. The results are copied using a system command.

Two important things to note:

  1. You have to do the set command before you change the jobname, otherwise your RST files will not work
  2. This version is written for windows, you need to use forward slashes and cp for Linux.

You can attach this to a MAPDL system or as a code snippet.