If you missed the presentation you can view a Recording here.
Or download a PDF of the presentation here:
As always, you can see which webinars are coming up, and view recordings of past webinars at:
If you missed the presentation you can view a Recording here.
Or download a PDF of the presentation here:
As always, you can see which webinars are coming up, and view recordings of past webinars at:
Unable to converge. Convergence Failure. Failure to Converge. Never nice words to see when you are trying to get your simulation done.
If you’ve encountered convergence failures while running nonlinear structural analyses in ANSYS Workbench Mechanical, this two part series is for you. What is a convergence failure? In a nutshell it means that there is too much imbalance in the system. The calculated reaction forces do not match the applied loads and even though the program tries hard to make changes to overcome the imbalances, it hasn’t been able to do so and stops. If we look at the Force residuals under Solution Information, we will see that the solver has been unable to get the force convergence residual, or imbalance force, to drop below the current criterion
Test model example: Newton Raphson Convergence Failure; Solution Stops
We won’t spend a lot of time here explaining the Newton-Raphson method, convergence, and residual plots here, since we wrote a Focus article back in 2002 which discusses them in more detail. The article begins on p. 7 at this link:
The context of that article was Mechanical APDL, but the article is directly relevant since solving in Workbench Mechanical is done in Mechanical APDL in batch mode.
In crayon terms, we want the purple line to drop below the blue line. When it doesn’t and the solver is out of options to keep trying, the solution stops and we get an error message.
Now what? The traditional knobs to turn are to increase the number of substeps, decrease contact stiffness if contact is involved, perhaps add more points to the plasticity curve, etc. But what if something else is the problem? How can we identify where the problem is?
In this part I article we will discuss how to plot the Newton-Raphson residuals as contour plots to see where in the model the highest force imbalances are located. Often this is useful information to help us figure out what is going on so we can take corrective action. First, be aware that we must turn on the Newton-Raphson residual plots prior to solving. That means you either have to turn them on and re-solve after a convergence failure, knowing that you’ll get the same failure again, or you need to clairvoyantly (or perhaps just prudently) turn on the residuals prior to attempting the initial solve. Why aren’t they on all the time, you ask? Most likely because they slow things down just a bit and also require a bit more disk space than otherwise, although if the solution runs to completion no Newton-Raphson residual plots are saved.
Here is how we turn them on. In the Details view for the Solution Information branch, change the Newton-Raphson Residuals setting from the default of zero to a nonzero number such as 3 or 4. That will continuously save the last 3 or 4 Newton-Raphson residual plots for viewing as contour plots after the solution has stopped due to a convergence failure.
After the solution has stopped, the Newton-Raphson residual plots will be available under the Solution Information branch.
The quantity plotted is actually the square root of the sum of the squares of the residuals in the global X, Y, and Z directions. So, the plots don’t show us direction information, but they do show where the residuals and hence the force imbalances are the largest. Below is an example. The region in red shows where the residuals are the highest. Since this is a model involving contact between two bodies, apparently the contact regions and specifically contact at the corners of the part on the left is the source of our convergence difficulties.
Newton-Raphson Residual Force Plot for the last attempted equilibrium iteration.
So, how do we use this information? In this case we now suspect that the contact regions, especially at the corners of the smaller part, are the problematic areas. Using this information we made two changes to the model.
First, we changed the Detection Method for the contact elements from Program Controlled (at the element Gauss points) to Nodal-Normal to Target. Many times when contact problems involve touching at corners, the robustness of the contact interface can be improved by changing the detection method from Gauss points to nodes.
Second, we reduced the contact stiffness by changing Normal Stiffness from Program Controlled (factor of 1.0) to a Manual setting of 0.2. Reducing the contact stiffness can help with contact convergence for a lot of problems. Too low of a stiffness value can cause problems too, but in this case the resulting penetration is still small so a value of 0.2 seems reasonable. When in doubt, a sensitivity study can be performed whereby you make changes to the contact stiffness value while tracking your results quantities of interest. As with most inputs you can vary, your results of interest should not be sensitive to contact stiffness.
These two changes allowed our test model to nicely converge for the full amount of load.
The Newton-Raphson Residual plots are always displayed on the original geometry, not the deflected geometry at version 14.0 of ANSYS Mechanical. If the deflections are large this can make it harder to ascertain what is causing the high residual values. In those cases, it can be helpful to compare the total deformation and stress plots for the unconverged solution, along with those plots for the last converged solution, with the 1.0 true scale on the deformation active. This will show the parts in their deflected state, and that can help in determining why the residuals are high at certain locations.
We recommend creating at least 3 residual plots (set in the details of Solution Information as described above). Sometimes the location of the imbalance can bounce around a bit from equilibrium iteration to equilibrium iteration, so having more than one or two plots to look at can be beneficial in determining problem locations.
Summing it up, the Newton-Raphson residual plots are one piece of information we can use to determine why we are having convergence difficulties. They can give us an indication of where the convergence difficulties are occurring in the model, and many times we can use that information to help us know what settings should be modified or what other changes should be made to the model to improve the convergence behavior.
In part II of this article, we’ll look at how to quickly use ANSYS Mechanical APDL to view the elements that have undergone too much deformation.
OK, it is Friday afternoon and if I do not write something soon the week will be missed. We did not do a seminar this week so I can not just post the notes and some comments from the webinar, bummer. All of the real tech support people at PADT have been busy with training, mentoring and doing tech support, so they did not kick anything out. So that leaves me to come up with something. So, as is usually with me, I looked for something I felt guilty or ashamed of. Because that is the way my brain works.
And I remembered that two posting ago I put out a piece of junk macro that printed out tables, as part of the second article on tables in APDL. Although it worked it was brute force and it used a bunch of *if statements to determine how many columns to write. Ugly.
While I was extruding that particular piece of bodily waste something in the back of my mind said that APDL had an undocumented command that would suppress a line-feed on a *VWRITE. This is what one does with ‘C’ and other languages invented after the 1970’s. If you suppress the line-feed, you can just loop over the number of columns.
Next step, go to the help and see if it is there is some clue as to if that tickle in my brain was valid. I found a posting on XANSYS from 2004… by some guy name Eric Miller… Go figure.
There are two descriptors that are not documented in the help: ‘/’ and ‘$’.
‘/’ adds a newline, and ‘$’ suppresses it. So if I want to write out the values in a 1D array all on one line but I don’t know how long the array is I can do:
myar(1) = 1,2,3,4,5,6,7,8,9,10
So, extrapolating this, we can rewrite the nothing-to-be-proud about old wrttbl.mac with
Have a great weekend!
Presentation PDF is here:
Zip file with the sample USERMAT.f and input file:
I was a bit confusing on state variables. The problem is with my use of them, not with the variables. The test model only had one integration point. My code is still not working right, the default USERMAT is overwriting my flag somewhere and I don’t have time to figure it out. It’s killing me but I have to do some real work.
But anyhow, my assertion that the state variables are per integration point is correct.
I am not aware of any way to use a debugger with ANSYS. There is nothing in the documentation, and to be honest, I’ve not used a real debugger in years. So there may be a way to do so, and see your routine in the debugger since you have the source code, but I have no idea on how to do that. Perhaps someone with more debugging experience can comment below.
Someone asked about other routines that are available and we ran out of time before I could go over them. Here is a list.
|UserElem.f||User Defined Element that use newer API|
|UEL100.f – UEL105.f
UEC100.f – UEC105.f
UEX100.f – UEX105.f
|User elements defined that access the program database directly|
|USEROU.f||Stores user-provided element output|
|USERAN.f||Modify orientation of material properties|
|USERRC.f||COMBIN37 (control/thermostat/spring/damper/resistor) user routine.|
|UEIMatx.f||Access to an elements matrix or load vector|
|UTHICK.f||Sets thickness at integration points|
|UsrFictive||Sets “fictive” temperature (I have no idea what that is)|
|UFLEX.f||Calculates pipe flexibility for PIPE288/289|
|UsrShift.f||Allows user to specify time shift|
|UserMat.f||User material models|
|UserHyper.f||User defined hyperelasticity models|
|UserCreep.f||User defined creep model|
|user_tbelastic.f||Allows definition of elastic stiffness at a given integration point based on user model. TB,ELASTIC,,,,USER|
|USERFC.f||User defined failure criteria|
|USERSWTRAIN.f||User defined swelling, for TB, SWELL,,,,USER|
|USERCK.f||Helper routine that passes material properties for a user material in|
|USERFRIC.f||User defined friction calculation. Not just friction but all values calculated in contact calculations with friction turned on.|
|USERFL.f||Changes scalar field values (temp, fluence, heat generation, moisture content, magnetic virtual displacement), by element.|
|USERPR.f||Calculates element pressure, by element|
|USERCV.f||Calculates element face convection.|
|USERFX.f||Calculates element face heat flux|
|USERCH.f||Calculates element face charge density surface values|
|USERFD.f||Computes complex load vectors for frequency domain logic|
|USERPE.f||Calculate the rotation of an elbow pipe element caused by internal pressure|
|Modifies the conduction, film coefficient, bulk temp for SURF151/152|
|userPartVelAcc.f||Ocean wave particle acceleration calculation for PIPE288/289|
|userPanelHydFor.f||Calcs hydrodynamic loading on SURF164 from ocean loading|
|USER01.f-USER10.f||Create your own ANSYS commands that are accessed through /UCMD,cmd,num where num refers to the subroutine number and cmd is the command name you want to assign it. Put this in your startxx.ans file to give regular access.|
About a month ago we published an article on “What Every User Should Know About Tables in ANSYS Mechanical APDL” At the end of that article we had a section on “Other Stuff” and expressed our hope to cover those subjects in the future. The future is now. If you are not very familiar with table arrays, make sure you review the previous article before delving into nesting and 4/5 dimension tables in this article.
By the way, the funky table at the end of the article got a lot of good feedback, so I’ve googled around and found some other interesting tables. The one here at the top is what you get if you google “complicated table”
As you will remember from memorizing the previous article, a common use for tables is the set them up to give you a value for a given “primary variable” that is determined by the solver at a given point in the solution. Possible primary variables are: TIME, FREQ, X, Y, Z, TEMP, VELOCITY, PRESSURE and SECTOR. But what if you want to use one of those primary variables to look up a value, then use that value to then interpolate a second value?
A good example is that you have a piece of rotating equipment and the value of the heat transfer coefficient (HF) is a function of RPM and the radius of a given element face. But RPM varies over time. What you can do is make the HF table point to and RPM table that is based on the primary variable time:
mycnv(1,1) = .25,4,10
mycnv(1,2) = .35,7,15
mycnv(1,3) = .45,10,28
This macro is missing stuff, like a model and selecting the nodes to apply the SF command to.
The tables look like this:
Table: mycnv RPM vs X
| 0.000 1.000 2.000
0.000 |0.2500 0.3500 0.4500
1000. | 4.000 7.000 10.00
0.2001E+08| 10.00 15.00 28.00
Table: rpm TIME vs
0.000 | 0.000
10.00 | 5.000
40.00 | 20.00
60.00 | 30.00
(We’ll cover the wrttbl macro below.)
So at a given substep, the program will take time and figure out what RPM needs to be. Then it will use RPM and the radius (X in CSYS 1) to figure out the convection coefficient for each node.
As you can imagine, you can get pretty sophisticated with this. The key is that the name of the table you use for the calculated value is input into the variables to interpolate on for the second table, using the *DIM command.
Another common use is scaling tables based on some value. Let say you have a pressure table and the total pressure is scaled over time, based on time. You would make a pressure table that is dependent on say X and y. It would have two planes. One with 0 values and one with the max values. Then you would make a scale table that scales from 0 to 1 based on time. It would look like this:
*DIM,pscl,table,5,,,time !Row label is CPTAB, the table of Cps
pscl(1,1) = .25,.5,1,1,.333
ptab(1,1,1) = 0,0,0,0
ptab(1,2,1) = 0,0,0,0
ptab(1,3,1) = 0,0,0,0
ptab(1,4,1) = 0,0,0,0
ptab(1,1,2) = 72,48,97,123
ptab(1,2,2) = 53,48,88,98
ptab(1,3,2) = 43,38,77,88
ptab(1,4,2) = 33,28,55,77
As always with tables, double check things and make sure you have your rows and columns correct. Start simple, and then add more detail. Testing out on a 2×2 or 3×3 tables is a good way to start.
Most users will simply use a one, two, or even three dimension array or table (row, column, plane). However, both arrays and tables support two more dimensions: books and shelves. Because this capability is a later addition to the program, it behaves a little differently. You need to add values for the size of the book (KMAX) and the shelf (MMAX) as well as variable names for each: VAR4 and VAR5
The first difference is in the *DIM command. For normal arrays and tables you use:
*DIM, Par, ARRAY, IMAX, JMAX, KMAX, Var1, Var2, Var3, CSYSID
*DIM, Par, TABLE, IMAX, JMAX, KMAX, Var1, Var2, Var3, CSYSID
For 4 dimension arrays or tables you use:
For 5 dimension arrays or tables you use:
It is important to be aware of this because if you look at the manual entry for *DIM it only lists the 3 dimension version of the command, and these variations are covered in the notes.
Once the array or table is defined you have to fill it using APDL commands, this size is not supported in the user interface. The same commands are used, but instead of supplying one, two or three indices values, you supply four or five.
The following is an example of defining a table in terms of location (X,Y,Z), Time, and Temperature. This is the most common usage of a five dimension table:
*dim,ldval,tab5,3,3,3,3,3,X,Y,Z,TIME,TEMP ! table
*taxis,ldval(1,1,1,1,1),1,-2.3,0,3.4 ! X Range
*taxis,ldval(1,1,1,1,1),2,-1.2,0,1.8 ! Y Range
*taxis,ldval(1,1,1,1,1),3,-3.6,0,4.5 ! Z Range
*taxis,ldval(1,1,1,1,1),4,0,5,10 ! Time Range
*taxis,ldval(1,1,1,1,1),5,32,320,500 ! Temp Range
!silly made up equation to fill the table with
ldval(ii,jj,kk,ll,mm) = ii*.123+jj/.2+ll*kk+mm*JJ*JJ
For simple 2D tables with up to 10 columns, I use a cheesy macro I wrote called wrttbl.mac. It was used above. It is a bit of a brute force method, because it has code blocks for from 0 to 10 columns. A more general approach would build the actual *VWRITE commands with *VWRITES… It should also be expanded to do Planes. Maybe for a future article.
Anyhow, here it is, maybe you will find it useful.
ttbl = arg1
fname = arg2
nmcl = nint((ncl*10)/2)
nmrw = nint(nrw/2)
('Table: ',A,' ',A,' vs ',A)
And with that, I think we have beaten the table topic to death.
PADT is proud to announce that it has added the VCollab 3D Visual Collaboration Software for CAE (http://www.vcollab.com) to its software product offerings. PADT will offer VCollab along with VCollab’s facilitating CAX file format to deliver on the growing need for smaller simulation result files and increased efficiency in data transfer to its customers in Arizona, New Mexico, Colorado, Utah and Nevada. You can read more at on our press release.
What does this mean to you the ANSYS user? Well it means you can share your models and results in 3D with others: over the web, imbedded in MS Word or PowerPoint, from within EKM, or as a stand alone file. The tool converts your monster ANSYS result file into a lightweight file that only has the results you want to share. We like it because of the small file size and the fact that we can send one 3D “image” instead of a bunch of different 2D images to our customers.
You can learn more about it at our next Webinar:
Using VCollab to Share 3D ANSYS Results
September 13, 2012
12:00 – 1:00 MST
You can also try it out yourself by signing up to get the free viewer:
Register and they will email you a login. Once you log in you can download the viewer (Download tab) and also look at some sample models they have.
Note: You need to set the following Environment Variable:
Variable : VCOLLAB_SKIP_OGL_DRIVER_CHECK
Value : 1
You can also look at the one we use in the Webinar:
We will be sharing more on this tool as time goes by.
We announced that we were a Geomagic reseller when we rolled out our 3D Laser and Cross Sectional Scanning hardware offerings. Although we added this as a tool for our scanning customers, we have found many ANSYS customers that are interested in it or that already had it in house.
If you don’t know Geomagic, it is a suite of tools that take scan or faceted (yes, meshes are included) and allows you to repair them, wrap them, compare them, or convert them to usable CAD solid geometry. Yes, this is the tool you have been looking for to take your distorted FEA mesh and convert it into a usable CAD model.
So we wanted to let everyone know that we are now certified to offer training on the Geomagic suite. As always, we can offer training when your want it and where you want it, or you can sign up for one of PADT’s scheduled classes. The first two are in October:
Click on the course names to get more information on the content and to register, or simply contact us at 480.813.4884 or email@example.com.
Look for some Focus articles on Geomagic, or a seminar for ANSYS users, later in the year when we get caught up on our backlog and Joe has some time to prepare something.
Recently a customer approached me and told me that he had a sketch in one DesignModeler database that needed to be copied over to another DesignModeler database and asked me if it would be possible to do so. My initial reaction was, “No way, dude be trippin’,” because that’s how I talk in professional settings. But, I really wasn’t ready to assert its impossibility without first digging into it a bit, so that’s what I did.
Clicking around the DesignModeler menus (Ever wonder how we ANSYS support professionals figure things out? Now you know.) I found something that had flown under my radar previously. Under the File menu are a couple of selections indicating the ability to write and read sketch scripts. Pay dirt.
So, what is it that these wonderful scripts can do for us? Let’s take a look. Say, for example, you have two separate sketches in two separate DesignModeler sessions. I have labeled these sessions “Face” and “Head.” See if you can figure out which is which.
(Side note: It may be hard to believe, but this is not the original geometry the customer was working with)
Now, keeping in mind that these are two completely different DesignModeler databases, how can I copy the Face sketch, including dimensions, and paste it on top of the Head sketch? The answer is simple. First highlight the DesignModeler plane containing the Face sketch.
Next, click File > Write Script: Sketch(es) of Active Plane. You will be prompted for a file name and location of the resulting jScript file. Specify those and click [Save].
Note that all of the sketches on the selected plane will be written to the jScript file. If there are any sketches you don’t want to keep, you can always delete them later.
Next, move over to the Head model. Highlight the plane you would like to copy the Face sketch to. In this case, it is the XYPlane again, but you can pick whatever plane you want; it doesn’t have to be the same plane between sessions. The sketch will maintain its position relative to the origin of whichever plane you select.
Next click File > Run Script and select the jScript file that was written previously. Click [Open].
More than likely, you will get a warning about modifying the feature number to avoid duplicates. This is normal. It simply means that it’s renumbering the imported sketch to avoid having, for example, two “Sketch1” objects. Click [OK].
You will now see the Face sketch, dimensions and all, overlaid on the Head sketch. The Sketch object has been renumbered and placed onto the XYPlane.
And, as you can see, everyone is happy.
You may have noticed there are several official service packs available for ANSYS 14.0. In case it’s not clear to you what each of these service packs is for, here is a brief explanation to hopefully allow you to determine which of them you may need for your particular application of ANSYS products.
ANSYS140.0.1: Service Pack 1:
This fixes a rare scenario in which the ANSYS Mechanical database can be overwritten with a zero size file on exiting ANSYS Workbench by clicking the close window icon. This is recommended for all Workbench Mechanical Users.
ANSYS140.0.3: Service Pack 3:
This fixes a problem causing a potential solver error for ANSYS Mechanical APDL ("classic") for large modal superposition harmonic analyses. The definition of large is on the order of half a million degrees of freedom. If you are an ANSYS Mechanical APDL user, this service pack is recommended.
ANSYS140.0.8: Service Pack 8:
This fixes a list of issues with ANSYS Icepak. If you are a user of Icepak 14.0, this service pack is recommended.
ANSYS140.0.10: Service Pack 10:
This fixes a performance (speed) issue with ANSYS Composite PrepPost 14.0. As of this writing the service pack is only available for Windows 64 bit platforms. This service pack also includes service pack 1.
All other service packs are available for Windows 32 bit, Windows 64 bit, and Linux 64 bit systems. All service packs and more info on the service packs can be obtained on the ANSYS Customer Portal in the software download area. Click on the hyperlink for a given product’s "Last Update" date. That will bring up documentation on the available service packs for that product.
This week went by very fast, and I never got time to do the more advanced article on tables to follow up on last week’s article. So I was going to give up till someone stopped by my office to ask a question and I thought my simple and clever answer would make a nice quick, but useful, posting.
What he need to do was apply fairly complicated loading over multiple substeps. Do some *get’s, calculate some stuff, then apply a load. I immediately thought of a trick we used in the early days of ANSYS Mechanical (before it was called ANSYS Mechanical) where we would put in a script that redefined the solve command as nall (*abbr,solve,nall). You then used your own code to do the solves.
This made us feel very smart and clever.
However, something in the corner of my brain was saying “dumb and silly.” So I fired up 14.0 and realized that my brain was right, you don’t have to trick ANSYS Mechanical any more. The developers now allow you to specify load steps and such for preprocessing command objects. I should know this because I did a seminar on APDL Command Objects. .
Darn no article for this week, it was already covered.
But just to make sure I looked through the PowerPoint and found that the ability wasn’t covered. Yipee! I have an article, now to stretch it out make it look important!
If you insert a command object into your model setup:
You end up with a Details view like so:
Under definition you can set “Step Selection Mode” This simply lets you determine if the APDL code in the command object is applied every load step (All), at the first (First), at the last (Last), or if the command object is only applied to a specific load step number (By Number).
If your complicated loading/modification to your model is the same commands for every load step, pick All and enter your commands. If it varies by load step in some way, you have two choices. You can write a set of commands for each load step, or you can write a macro that uses a *get,nmstp,active,,solu,ncmls and then use logic to figure out what you need to do.
So, pretty simple, but it opens up a lot of possibilities when you need to do some simple tweaks during a multi-step solve.
There, now I don’t feel like a looser for not doing an article this week.
I was having a discussion with a user who is very experienced with a FEA tool other than ANSYS. He wanted to define some properties with respect to time and his rotational speed and wanted to know how hard it would be to write a custom routine in ANSYS to do that. I immediately explained that it was not that hard, as long as you have the right compiler. Then I realized that you did not need to compile any code. Unlike that other software, we have tables in ANSYS and you can use those to interpolate data relative to some other value. And, now that it is Friday morning and we still do not have a FOCUS article for the week, I thought it would be a good time to review the basics of Tables in APDL.
ANSYS Mechanical (Workbench) users, do not leave and go back to reading TMZ. This is useful to you as well because you can use code snippets in ANSYS Mechanical to define some very sophisticated loads without ever getting into Mechanical APDL. One of those cool powerful things you can do in Mechanical. In fact, if you look at the input file that ANSYS Mechanical sends to the solver, it is often full of tables that ANSYS Mechanical makes.
This article will just touch on the simple aspects of tables that every user should know. There is a lot more you can do with tables, but we will save that for future articles.
The APDL language has three type of parameters: variables (single numbers or 8 character strings), arrays, and tables. variables and arrays are just like variables and arrays in most programming languages. But tables are unique in that the indices are real numbers rather than integers. And when you refer to a value in a table the program does a linear interpolation between the numbers you supply to get the value at that location. Think of it as a graph where instead of points you have a line:
What makes it even better, is that the table can be multiple dimensions. So you can make a value dependent on a location in 3D space, val(x,y,z), space and time, val(x,y,z,t), or even some input you need to use, val(x,y,z,t,myVal).
You get an interpolated value by simply using it in a formula:
x = 2.4
y = 1.66
z = 23.5
frc = frc_tbl(x,y,z)
Also, many commands in ANSYS Mechanical APDL take a table as an argument. And the solver will input proper index values at solve time. The simples example of this is a nodal force using the F command:
For each substep, the solver will interpolate a force value for node 47 in the X direction based the value of things like time, frequency, position, temp, and such for the current substep. More on how to define what values to use as an index below.
One other key thing to know about tables before we get into the details is the way they work. What ANSYS does is take an actual array, and add a 0 column, row or plane to the array. So instead of going from 1 to 10, the array goes from 0 to 10. And the index values are stored in this 0 row, column, or plane. So to see the values using the *STATUS command, you have to tell it to start listing at 0 with the IMIN, JMIN, or KMIN arguments:
Another good way to look at a table is using the *VEDIT (Parameters->Array Parameters->Define/Edit->Edit.)
The hardest part of defining a table is defining the index and values. Arrays are simple, you just define you r size with a *DIM and then supply a value for each integer index value:
val(1) = 12.4,15.6,18.5,12.4,12.4,5,3.2
For tables, you need three steps: define the table with *DIM, define the indices (the axes), then provide the values.
val(1) = 12.4,15.6,18.5,12.4,12.4,5,3.2
Note that in the *DIM command, you have to specify that this is a table with TABLE. For array’s you can say ARRAY or leave it blank, because ARRAY is the default.
The next command, *TAXIS, is the important one. It does not call several cabs to pick you up. It defines the Table AXIS… get it, TAXIS. The first argument is the name of the table you want to fill, with the index put in for the row you want to start on, and the second is the index you want to fill. Then you give the actual values.
Finally we supply the actual values just like in an array, but each value corresponds to the index values specified in the *TAXIS command.
The above example results in:
This example is for a 1D table. A 3D table works the same, you just need to define 3 axes and 3 columns of values. Note that the first argument on the *TAXIS command is the column number that the axis refers to.
temptab(1,1,1) = 10,100,10
temptab(1,2,1) = 12,150,10
temptab(1,3,1) = 10,90,7
temptab(1,1,2) = 12,120,12
temptab(1,2,2) = 15,180,15
temptab(1,3,2) = 17,90,12
temptab(1,1,3) = 20,200,20
temptab(1,2,3) = 22,250,20
temptab(1,3,3) = 20,290,27
This will produce:
If you find the code a bit confusing, we recommend that you use Parameters->Array Parameters->Define/Edit->Add… to create your tables, then look at the log file to get the commands.
Using Tables with Loads
The real value of tables is their use with commands that accept a table as a value, and this is usually some sort of load. The help for a given command will tell you if it takes a table as an argument. If it does not, simply put the command in a *do-loop.
When you specify a table, you need to tell the command interpreter that it is a table and not variable or a string by placing the command in side percent signs: f,frc_nodes ,fx ,%fx_load%.
But how do you tell the solver what solver values your indices refer to? If you want the force applied based on the X,Y,Z position of the nodes in the component frc_nodes, you need to say which column in your table is X, Y, and Z. You do that with the *DIM command:
*DIM, Par, Type, IMAX, JMAX, KMAX, Var1, Var2, Var3, CSYSID
Var1, Var2, and Var3 are predefined keywords that are called Primary Variables. The possible values are:
|X||X location of entity|
|Y||y location of entity|
|Z||z location of entity|
|SECTOR||Cyclic sector number|
So to define loads that vary with Z position and time you would do:
val(1,1) = 12.4,17,10.5
At each substep the program will go through each node in FRCNDS and get its Z location and the current time and interpolate a force and apply it to that node. I do not know about you, but I think that is pretty slick.
The obvious next question is how do I deal with a different coordinate system? The last argument on *DIM is CSYSID. You supply a local coordinate system number here and the program will use that coordinate system to figure out the position of the entity it is applying a load to.
We strongly recommend you look at the *DIM and *TAXIS commands in the help. Also read section 3.10 of the ANSYS Parametric Design Language Guide, specifically the section on Table Type Array Parameters.
Some other things you can do with tables that we hope to cover in the future, but that you can also figure out on you own using the help are:
// Basic Analysis Guide // 2. Loading // 2.5. Applying Loads
And we will finish with a picture of a really cool table and bench I found on line: I want to get this for my patio.
Maybe you’ve seen AQWA show up in the list of ANSYS products to be installed on your computer, or maybe you’ve seen it as a topic in the ANSYS Help System and you otherwise wondered about it. Is it related to Aqua Man or perhaps Aqua Lung? Not at all. If you are not familiar with it, AQWA is a tool for simulating wave and current as well as wind loads on marine vessels and structures.
Truthfully, although we are located in the Sonoran Desert, we have some great lakes within a short drive of Phoenix, let alone Tempe Town Lake just a few miles from PADT, and lakes Powell and Mead up on our northern and western borders with Utah and Nevada offer miles and miles of incredible scenery. However, most of our rivers are dammed for water storage and irrigation so it’s not uncommon to see river beds with no water in them for most of the year. A standard joke is that Arizona is the place where rivers and bodies of water are not associated with each other.
The bottom of the Salt River, aka Rio Salado, which flows through Phoenix (Sometimes)
The Nav System Knows it as a River
Yes, it does rain in Phoenix. Just not often. This storm caused over an inch of rain in some places:
This is more of a typical day. No rain in sight:
You may be wondering why we have an interest in AQWA here in the Sonoran Desert. The short answer is that we support an organization working on alternative energy sources, including offshore wave power. As a result, we’ve had to become familiar with the ANSYS AQWA suite of tools.
Incident Waves on a Moving Ship:
At version 14.0, the main part of AQWA, hydrodynamic diffraction, is integrated with ANSYS Workbench. In a hydrodynamic diffraction analysis, we are calculating the response on our structure due to incoming and receding waves. The effects on the water due to its interaction with the structure are also included. It’s also possible to perform a hydrodynamic time response analysis within the Workbench framework. Interaction with permanent structures such as piers and breakwaters can be included as well.
The use of Workbench means we can use ANSYS DesignModeler to construct and edit our geometry, including a slice at the waterline and formation of a multi-body part, both of which are needed for AQWA. It is somewhat integrated with Workbench Mechanical, in that it’s possible to map pressure and inertia loads from AQWA into Mechanical for a detailed structural analysis, but it’s somewhat of a manual process currently. For those familiar with the ANSYS APDL command language, it’s fairly straightforward.
Geometry Split at the Water Line in DesignModeler:
AQWA can also be run in stand-alone mode, which opens up additional capabilities while still taking advantage of DesignModeler surface geometry or another source. The various modules have creative names such as AQWA-Line, AQWA-Librium, AQWA-Fer, AQWA-Drift, and AQWA-Naut. Besides hydrodynamic diffraction, one can look at the effects of mooring lines, cables and tethers and varying wave and wind loads on structures. Special elements are included which facilitate the simulation of ‘stingers’ or articulated trusses which are used to connect underwater piping to floating vessels. Fenders can also be modeled to allow for interaction between floating and floating or floating and permanent structures that may come into or out of contact.
Geometry of the structures modeled consists of surface models which are meshed with shell elements. Meshes must be relatively coarse compared to what most of us who normally perform structural analyses are used to. Small geometric details usually need to be omitted to keep the mesh sizes down, but that’s not really a problem as we are trying to accurately predict interaction between the fluid and the structures, not stress concentrations or other localized results within AQWA.
In addition to plots and animations of interacting waves and pressure distributions, many other results quantities are available including cable forces, RAO’s (response amplitude operators), drift coefficients, shear force and bending moments, and other quantities used in the industry. These quantities are useful to those developing sea-going vessels as well as for those in the oil and gas industry involved in developing Floating Production, Storage, and Offloading (FPSO) structures and Tension Leg Platforms (TLP’s), etc.
Forces on Two Mooring Lines vs. Time:
Floating Structure Lateral Position vs. Time:
If any of this looks like a tool that would be useful for the types of projects you work on, by all means contact your local ANSYS provider for more information. You’ll want to plan on taking the AQWA training class, which we have found very useful.
One of the lakes along the Salt River. Indeed there is water in the desert, if no ocean:
This article is the eagerly awaited fourth and final installment in my series on interacting with nodes in ANSYS Mechanical. To review, the previous three articles covered picking your nodes, creating named selections from nodes, and applying boundary conditions to nodes. I know some of you were wondering why it took a while for this final article to come out. Well, I’d been sent to my home state of Indiana for business and decided to take a few extra days to visit relatives—living and not-so-living.
Now on to business. Our discussions so far have centered on preprocessing and solution processing operations with nodes. Now we’ll conclude the series by covering postprocessing operations with nodes in Mechanical. Much the same way that you can scope boundary conditions to nodes, you can also scope results to nodes. There is one key difference however: whereas nodal boundary conditions can only be scoped to named selections, nodal results can be scope to geometry or named selections.
Scoping results to nodes based on geometry selection is accomplished using the same procedure as scoping results to any other geometry: simply select the nodes of interest, and insert results.
Likewise, for named selections, simply insert the results object of interest, set the Scoping Method to Named Selection and choose the appropriate named selection.
Does something appear a bit unusual about that last figure? Notice that the results are plotted as continuous contours, with the nodes emphasized, rather than just appearing as discrete points. When all of the nodes on an element are selected, such as in this example, the results are displayed as a continuous contour across the face. Here’s an example showing what happens when some element faces have all their nodes selected, and others have only a few.
Beyond the standard analysis results, you can perform some additional nodal orientation verification as well. Remember how in the third article in this series I sent the Mechanical modal over to Mechanical APDL and turned on the nodal coordinate systems there to verify their orientations? Now you do, because I linked you to it. Well, as it turns out, you can get the same information in Mechanical. Let’s see how.
As an example we’ll start with the same valve with a cylindrical coordinate coordinate system located at the center of the outlet flange. The nodes on the outlet flange face (Named Selection: Outlet Flange Nodes) have been rotated into this cylindrical coordinate system and a 0.01” displacement applied to them in the Y (theta) direction. The inlet flange is fixed.
After solving the model, highlight the Solution branch and click on the Coordinate Systems pulldown, way on over to the right of the Solution toolbar, next to the Command Snippet button.
Using this pulldown menu, you can display nodal coordinate triads and nodal rotation angles. The Nodal Triads pick displays the nodal coordinate systems, equivalent to executing /PSYMB,NDIR,1 in Mechanical APDL.
The Nodal Euler Angles display the amount of nodal rotation in each plane from the original position. Here’s a plot of the Nodal Euler XY Angles of the outlet flange nodes.
Wait a second. Don’t those contours seem a little “off” to you? They’re not lined up radially, and the zero and 180 degree rotation values aren’t quite located where I expect them to be. Wait, I think I know what the problem is. Let’s set the displacement scaling to 0.0 (Undeformed) and see what happens.
There, that’s better.
Note that you can also display element triads and Euler angles, for rotated element coordinate systems, but that’s a topic for another day.
This completes the nodal interaction series for R14.0 ANSYS Mechanical. We will be sure to keep you informed of further improvements to finite element interaction capabilities in Mechanical as future versions are released.
There is a folder with a big fat exclamation point on the top of the Solutions branch in ANSYS Mechanical. It is called “Solution Information.” Most users click on it after their run is done and maybe look at the output from the ANSYS Mechanical APDL solve.
And it is very handy to check your output when your job is done:
But this feature has an exclamation point on its folder icon for a reason! It is a very useful tool! While doing tech support we have found that users often do not take advantage of the information displayed here, and if they did so their ANSYS Mechanical experiences would be more efficient and even more enjoyable.
When you click on the Solution Information branch in Solution, the graphics window turns to the worksheet window and you see Solver Output. This is the jobname.out file that ANSYS Mechanical APDL creates as it solves, and it is full of useful information. The window updates at a user defined interval, the default of 2.5 seconds seems to work well.
It is a good idea, even for a static run, to watch this window as things solve. It tells you where the solver is in the solver process, shows any warnings that might pop up, and lists the key information about your model and solver settings.
At first the information may seem a bit overwhelming. But give it time, study it, understand what each piece of information is and what it is telling you. Users who watch and understand the Solver Output when they solve understand their models better, and debug problems much faster.
The down side of the solver listing is that it is a text file. Text files are great for showing information at a certain portions of your run, but are not so great for comparing multiple points. But graphs are. And the same command can be changed to show all sorts of useful information about non-linear runs.
The list of available graphs varies depending on what type of solve you are doing. The most common values to look at are the Force Convergence for structural.
Take a look at this image. As you can see there are two graphs. The top one plots the convergence information you want to see vs. the number of iterations. The bottom graph shows time vs cumulative iterations. Notice that there is data being graphed, force convergence and criteria in this case. But there are also vertical dashed lines. These give you feedback on what events happen and at what iteration they occurred. Mostly they tell you that a substep or a load step converged.
You can watch these non-linear graphs while your model is running, or after the run to see what actually happened. I like to watch them as I solve because, honestly, it seems like the runs go faster. You find yourself watching that magenta line go up and down hoping it will go under the light blue line, and cheering when it does.
Take a look at the other types of non-linear graphs you can view and think about the impact of the data towards your run. As an example, if you see a lot of vertical lines indicating that you are bisecting, then you should look at setting up more substeps on each loadstep. The same thing if you see the convergence taking a long time. Such information can not only help converge a model that is having problems, but it can help you set up future runs such that they converge faster.
If you click on an item that there is no data for, you get a nice “No data to display” message. You will also get this before the data is available.
When you click on the Solution Information branch you will notice a “Solution Information” ribbon bar show up at the top of the window.
This allows you to define information you want to track while solving, things like displacement, gap on contacts, or energy. The values update as the problem is being solved, providing some nice insight into what your model is doing.
To use it, RMB on Solution Information or pull down the Result Tracker menu. Only results that are applicable to your solve will be available. Once you pick the ones you want, you need to specify the geometry you want to apply it to, if applicable. Usually it needs to be a vertex or a contact/joint. Do this in the normal way then fill out the rest of the detail view. As an example, if we want the deflection on the corner of an object, you pick the vertex on the corner then specify the axis you want the information in.
Note: You can not add a result tracker object during or after a solve, you have to do it up before you solve. So do not think about using this capability as a probe.
You can select as many of the objects as you want and plot them all at the same time, which is very handy. Once the run is done, you can save the graph as an image or export the data to a comma delimited file or as an Excel file.
We recommend you always set up a Result Tracker for tricky contact pairs and for any significant deflection that tells you a lot about your model.
The last feature in the Solution Information branch is really not solution information, but it kind of is. If you click on the branch you will notice a “FE Connection Visibility” area in the detail view. You will also find a “Graphics” tab under the Worksheet tab:
You use these tools to see things like beams, constraints and springs that are added to your model before the solve in ANSYS Mechanical APDL. So they can only really be seen as post processing entities. By default, all types are shown. But you can change the selection under “Display” in the details view to just show specific ones. You can also change the thickness of the display and do lines or points.
What is especially important about this is that beams, Constraint Equations and springs that you add in code snippets will also show up.
It is probably true that you could use ANSYS mechanical your whole career and never use this feature. but your career will be much more stressful and much less enjoyable than if just make their use part of your normal everyday process. It can save hours of trial and error debugging.
Plus, the reality is that while you are solving you could watch Justin Bieber videos on YouTube, or you can watch your model converge. That sounds like a much better way to go… watching the model convergence, of course… yea… cause Justin Bieber is lame… and… well, you know.