First Look: Pumpkin Launch 2012

For a couple of years now, PADT has had a tradition of shooting off pumpkin mortars on Halloween.  Originally we took dry ice, sealed it with some water in a 2 Liter bottle, put it in a tube with a pumpkin on top and “bang-whooosh” a pumpkin goes a flying.

Being engineers, we have to improve on the process… this year we used foam wadding, put cameras inside foam “pumpkins” and tried launching an ice pumpkin.  Here is the first attempt:

 

Pumpkin Launch

Look for more videos tomorrow.

Webinar Info: Getting Started with ANSYS Engineering Knowledge Manager (EKM)

imageLast Thursday (10/25/2012) Clinton Smith gave a well attended webinar sharing his experience getting the Engineering Knowledge Manager (EKM) up and running for him and how he used it on a project. As promised, the slides from that presentation and a link to the recording can be found here:

PDF of Presentation:

The Recording: https://padtincevents.webex.com/padtincevents/lsr.php?AT=pb&SP=EC&rID=5952687&rKey=eefe3ba0d2f0cbc6

Webinar Info: An Example of Moving Mesh Modeling of a Valve

imageLast week Clinton Smith gave a webinar showing an example of using moving meshes with ANSYS FLUENT.

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:

padtincevents.webex.com.

Suppressing New-Line Characters in APDL, and a Better WRTTBL.mac

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:

*dim,myar,,10
myar(1) = 1,2,3,4,5,6,7,8,9,10
*get,nrw,parm,myar,dim,X

*cfopen,foo1.txt

*do,i,1,nrw
*vlen,1
*vwrite,myar(i)
(g16.9,$)
*enddo
*vwrite
(x)
*cfclose
 
This ends up creating foo1.txt:

image

So, extrapolating this, we can rewrite the nothing-to-be-proud about old wrttbl.mac with

 

ttbl = arg1      ! Get the name of the table you want to write

fname = arg2     ! get the name of the file to write to

 

*get,nrw,parm,%ttbl%,dim,X         ! Get the size of the table

*get,ncl,parm,%ttbl%,dim,Y

*get,xax,parm,%ttbl%,var,1         ! Get the names of the columns

*get,yax,parm,%ttbl%,var,2

 

*cfopen,%fname%    !Open the file

 

*vwrite,ttbl,xax,yax    ! Write a header (note / to add a line)

('Table: ',A,' ',A,' vs ',A,/) 

 

*vwrite         ! write 10 spaces, then don't write a new line by using $

('          |',$)

 

*do,jj,1,ncl ! Loop on each column, writing out the column value ($ again)

    *vlen,1

    *vwrite,%ttbl%(0,jj)

    (g10.4,$)

*enddo

*vwrite    !You need a line feed now that you are done, just write a space

(' ')

*vwrite    !Write a line of  dashes to seperate the header, with a pipe

(10x,'|',$)   ! to seperate the row values

*do,jj,1,ncl

    *vwrite

    (10('-'),$)

*enddo

*vwrite

(' ')

 

*do,ii,1,nrw    !Now write the values, looping on each row, then each column

    *vlen,1

    *vwrite,%ttbl%(ii,0)

    (g10.4,'|',$) 

    *do,jj,1,ncl

        *vlen,1

        *vwrite,%ttbl%(ii,jj)

        (g10.4,$) 

    *enddo

    *vwrite

    (' ')

*enddo

 

*cfclose

Have a great weekend!

Webinar Info: Writing and Compiling a Custom Material Property in ANSYS Mechanical APDL

imageDuring our webinar held at noon on 9/27/2012 we promised to provide a link to the recording, a PDF of the PowerPoint, and some answers to a few questions.  Here is that information:

Files

Presentation PDF is here:

Zip file with the sample USERMAT.f and input file:

 

imageState Variables

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.

Debugging

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.

Other UPF’s

Someone asked about other routines that are available and we ran out of time before I could go over them.  Here is a list.

ELEMENTS
UserElem.f User Defined Element that use newer API
UEL100.f – UEL105.f
UEC100.f – UEC105.f
UEX100.f – UEX105.f
UEP100.f-UEP105.f
USERTR.f
USERAC.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
Materials
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.
LOADS
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
USRSURF116.f
USER116Cond.f
USER116Hf.f
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
USER Commands
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.

Other Stuff Every User Should Know about Tables in ANSYS Mechanical APDL: Nesting and 4 or 5 Dimension Tables

complicated table design

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”

Nested Tables

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:

*DIM,MYCNV,TABLE,3,3,,RPM,X,,1
*taxis,mycnv(1,1),1,0,1000,20.01e6
*taxis,mycnv(1,1),2,0,1,2
mycnv(1,1) = .25,4,10
mycnv(1,2) = .35,7,15
mycnv(1,3) = .45,10,28

*DIM,RPM,TABLE,4,1,1,TIME
RPM(1,0)=0.0,10.0,40.0,60.0
RPM(1,1)=0.0,5.0,20.0,30.0

wrttbl,'mycnv','foo4.txt'
wrttbl, 'rpm','foo5.txt'

SF,ALL,CONV,%mycnv%

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

and

Table: rpm      TIME     vs         

|0.7889E-30
|----------
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
*taxis,pscl(1,1),1,0,1,5,10,30
pscl(1,1) = .25,.5,1,1,.333

*DIM,ptab,TABLE,4,4,2,X,Y,pscl
*taxis,ptab(1,1),1,0,1.35,2.75
*taxis,ptab(1,1),2,-7.2,-3.2,6.5,10.6
*taxis,ptab(1,1),3,0,1
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

SF,ALL,PRESS,%ptab%

 

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.

4 and 5 Dimension Arrays and Tables

 
This section applies to both arrays and tables, so it is a bit beyond the scope of the title, but I hope you will forgive me.

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:

*DIM,Par,ARR4,IMAX,JMAX,KMAX,LMAX,Var1,Var2,Var3,Var4,CSYSID
*DIM,Par,TAB4,IMAX,JMAX,KMAX,LMAX,Var1,Var2,Var3,Var4,CSYSID

For 5 dimension arrays or tables you use:

*DIM,Par,ARR5,IMAX,JMAX,KMAX,LMAX,MMAX,Var1,Var2,Var3,Var4,Var5,CSYSID
*DIM,Par,TAB5,IMAX,JMAX,KMAX,LMAX,MMAX,Var1,Var2,Var3,Var4,Var5,CSYSID

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

*do,ii,1,3
*do,jj,1,3
*do,kk,1,3
*do,ll,1,3
*do,mm,1,3
!silly made up equation to fill the table with
ldval(ii,jj,kk,ll,mm) = ii*.123+jj/.2+ll*kk+mm*JJ*JJ
*enddo
*enddo
*enddo
*enddo
*enddo

sancal-elipse-floating-coffee-table-rafa-garcia-11Writing a Table to a File

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
*get,nrw,parm,%ttbl%,dim,X
*get,ncl,parm,%ttbl%,dim,Y
*get,xax,parm,%ttbl%,var,1
*get,yax,parm,%ttbl%,var,2

nmcl = nint((ncl*10)/2)
nmrw = nint(nrw/2)

*cfopen,%fname%

*vwrite,ttbl,xax,yax
('Table: ',A,' ',A,' vs ',A)
*vwrite,
(x)
*if,ncl,eq,1,then
*vlen,1
*vwrite,%ttbl%(0,1)
(10x,'|',10g10.4)
*vwrite
(10x,'|',10('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii ,1)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,2,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2)
(10x,'|',10g10.4)
*vwrite
(10x,'|',20('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,3,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3)
(10x,'|',10g10.4)
*vwrite
(10x,'|',30('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,4,then
/gopr
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4)
(10x,'|',10g10.4)
*vwrite
(10x,'|',40('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,5,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5)
(10x,'|',10g10.4)
*vwrite
(10x,'|',50('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,6,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5),%ttbl%(0,6)
(10x,'|',10g10.4)
*vwrite
(10x,'|',60('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5),%ttbl%(ii,6)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,7,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5),%ttbl%(0,6),%ttbl%(0,7)
(10x,'|',10g10.4)
*vwrite
(10x,'|',70('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5),%ttbl%(ii,6),%ttbl%(ii,7)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,8,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5),%ttbl%(0,6),%ttbl%(0,7),%ttbl%(0,8)
(10x,'|',10g10.4)
*vwrite
(10x,'|',80('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5),%ttbl%(ii,6),%ttbl%(ii,7),%ttbl%(ii,8)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,9,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5),%ttbl%(0,6),%ttbl%(0,7),%ttbl%(0,8),%ttbl%(0,9)
(10x,'|',10g10.4)
*vwrite
(10x,'|',90('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5),%ttbl%(ii,6),%ttbl%(ii,7),%ttbl%(ii,8),%ttbl%(ii,9)
(g10.4,'|',10g10.4)
*enddo
*endif
*if,ncl,eq,10,then
*vlen,1
*vwrite,%ttbl%(0,1),%ttbl%(0,2),%ttbl%(0,3),%ttbl%(0,4),%ttbl%(0,5),%ttbl%(0,6),%ttbl%(0,7),%ttbl%(0,8),%ttbl%(0,9),%ttbl%(0,10)
(10x,'|',10g10.4)
*vwrite
(10x,'|',100('-')) |
*do,ii,1,nrw
*vlen,1
*vwrite,%ttbl%(ii,0),%ttbl%(ii,1),%ttbl%(ii,2),%ttbl%(ii,3),%ttbl%(ii,4),%ttbl%(ii,5),%ttbl%(ii,6),%ttbl%(ii,7),%ttbl%(ii,8),%ttbl%(ii,9),%ttbl%(ii,10)
(g10.4,'|',10g10.4)
*enddo
*endif
*cfclose

And with that, I think we have beaten the table topic to death.

naturalistic-curved-wood-table-design-z

Get to Know VCollab, and Geomagic Training

VCollab_Shaded_Logo_FinalPADT 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.

imageYou 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:

http://www.marechi.com

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.

Geomagic_200x42We 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:

10/17/2012 – 10/19/2012      Geomagic Studio     PADT’s Tempe Office
10/22/2012 – 10/24/2012      Geomagic Qualify   PADT’s Tempe Office

Click on the course names to get more information on the content and to register, or simply contact us at 480.813.4884 or training@padtinc.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.

Running an APDL Command Snippet for Every Load Step in ANSYS Mechanical

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:

image

You end up with a Details view like so:

image

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.

What Every User Should Know About Tables in ANSYS Mechanical APDL

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 Basics

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:

image

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:

f,47,fx,%frc_tbl%

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:

*stat,frc_tbl,,,0

Another good way to look at a table is using the *VEDIT (Parameters->Array Parameters->Define/Edit->Edit.)

image

Defining a Table

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:

*dim,val,,7
val(1) = 12.4,15.6,18.5,12.4,12.4,5,3.2

Produces:

image

and:

image

For tables, you need three steps: define the table with *DIM, define the indices (the axes), then provide the values.

*dim,val,table,7  
*taxis,val(1),1,1.3,2.4,3.1,4.6,5.2,5.9,7.0
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:

image

and

image

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.

*dim,temptab,table,3,3,3
*taxis,temptab(1,1,1),1,0,5,10
*taxis,temptab(1,1,1),2,0,5,10
*taxis,temptab(1,1,1),3,0,5,10
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:

image

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:

TIME Time
FREQ Frequency
X X location of entity
Y y location of entity
Z z location of entity
TEMP Temperature
VELOCITY Velocity
Pressure PRESSURE
SECTOR Cyclic sector number

So to define loads that vary with Z position and time you would do:

*dim,val,table,3,3,,Z,TIME
*taxis,val(1),1,0,37,25.4
*taxis,val(1),2,0,.04,1
val(1,1) = 12.4,17,10.5
val(1,2) =8.3,7.4,12.8
val(1,3)=15.3,10.2,9.4
f,frcnds,fx,%val%

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.

Other Stuff

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:

  • You can create 4 and 5 dimension tables using TAB4 and TAB5 for TYPE in the *DIM command.  Other things need to be done as well, it gets complicated. You can find an example at:

    // Basic Analysis Guide // 2. Loading // 2.5. Applying Loads

  • You can nest tables inside tables.  So you can have one table calculate a value based on primary values (X,Y,Z, FREQ, TIME, etc) then use the result of that interpolation to interpolate from another table.   One use of this would be if a load varies with rotational velocity, and rotational velocity varies with time.  So you define an RPM table that is dependent on TIME, then use the table to get a load.  (maybe that will be next weeks article…)

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.

smooth 4 660x396

Solution Information: Monitoring your Solves in ANSYS Mechanical

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. 

image

And it is very handy to check your output when your job is done:

image

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.

Solver Output

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.

Non-Linear Graphs

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.

image

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. 

image

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.

image

Result Tracker

When you click on the Solution Information branch you will notice a “Solution Information” ribbon bar show up at the top of the window. 

image

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. 

image

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.

FE Connection Visibility

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:

image

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.

To see the entities, simply click on the Graphics tab:image

Conclusions and Recommendations

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.

image

Surface Projection Based Contact Detection

The ANSYS Mechanical APDL solver has a lot of contact options.  KEYOPT(12) this and KEYOPT(4) that.  I’m sure we all read Chapter 3.9 of the Contact Technology Guide to understand and remind ourselves on all these options.  I know here at PADT we always do so on the third Tuesday of every month… OK, maybe not.

But as fate would have it I was looking something up in there the other month and came across one of the newer options: Surface Projection Based Contact.  It is on of those little options that can make a big difference, so I thought I would put it on the list of potential Focus articles, and it just bubbled to the top.

Contact and Contact Detection

The way contact works in an FEA program is that you define a contact and a target. The program goes in and calculates if a point on the contact surface is near, touching, or inside the surface or point that is the target. If they are touching or inside forces are calculated acting on the contact points in the normal and tangential (friction) directions.  You use a slew of options to determine what that algorithm looks like. But hey all need to know what the gap or penetration is between the contact and target surfaces.

What is important for this article is how the program chooses those contact points to look at and, if needed, calculate forces on.

The default (KEYOPT(4) =0) is to use the gauss points on the elements.  Here is a great illustration from the online help:

image

Gauss points are good because there are more per element than nodes and calculations are done at the gauss points anyhow. The down side is that if you have a lot of curvature or even a corner, the true surface of your contacting part can penetrate into the target.

For those times when you do need to control things at the nodes, you can use KEYOPT(4) = 1 or 2. 

image

The down side is that the program now has to do a lot more calculations to make things happen at the nodes, and it has to calculate normals for the contact or target surface. Plus there are fewer points.  But the worst thing that can happen is node drop off if your mesh is not refined enough:

image

KEYOPT(4) = 3

Sometimes using points for contact results can cause problems. The node penetration or drop off being good example. it can also be an issue if there is a lot of “overhang” on an element.  So the developers at ANSYS have added a third option, the Surface Projection Based Contact Method, or KEYOPT(4) = 3.  What the method does is look at the element faces on each side of the pair, contact and target, and calculate the union of each.  If we look at the following example you can see it.  The green mesh are the contact surface elements, the cyan mesh is the target.  If we put them on top of each other, each unique area becomes a surface projected contact area, shown in the third image.

 

 image             image

image

So instead of calculating penetration/gap at each integration point or node, it calculates an average value for each overlapping area.  This can really make a big difference when you have the contact hanging off of the target, as shown in this illustration:

image

Advantages

So the three big advantages of this approach are:

  1. In most cases it provides a more accurate calculation of contact traction and stresses for the underlying elements.
  2. It is less sensitive to which side you designate as the target and which ones you designate as the contact surface. This is because you end up with the same projected areas.
  3. Moment equilibrium is satisfied if there is an offset between the target and contact surface and friction is turned on.
  4. Contact forces do not “jump” when a contact node slides off of the edge of a target surface.

Disadvantages

No surprise, it is not perfect or it would be the new default. The disadvantages are:

  1. The method is computationally more expensive because you usually have more contact areas then you would have contact points with the other method, especially if the target mesh is refined giving you more areas.
  2. The penetration or gab is an average value so when a model has corner or edge contact, the nodes on the edge or corner will penetrate into the target surface.  This is similar to what you see with the gauss point detection method. More refinement usually solves this.
  3. Free thermal surfaces don’t work with it. (What is a free thermal surface, I forgot as well.  It is a feature in thermal contact, Chapter 7.1 of the Contact Technology Guide. It is now on the Focus to-do articles list)
  4. You can not use a primitive for a rigid target. This makes sense if you think about it. If you use a primitive there are no element faces to find the overlap on.
  5. 3D contact and target elements can not have partially dropped midside nodes.  They either all have to be there or none.

ANSYS Mechanical

Although we have been talking about how things work in the solver, and the KEYOPTs used in Mechanical APDL, you can still access this through ANSYS Mechanical.  Any contact par will have an Advanced portion of its details view. In there you can access most of the KEYOPTs, including the Detection method, which is KEYOPT(4).

image

And here is the drop down for Detection Method. The last one, Nodal-Projection Normal from Contact is actually Surface Based Contact Projection:

 

image

Recommendations

The best way to get a feel for this is to find a couple of models you have already run with one of the other contact methods and run them with this option turned on and take a look at run time per iteration,  number of iterations for convergence and the resulting stresses in the contact area.    If you have flat, fairly refined contact/target meshes with no overhanging, you should just see things take longer.  But if you do have a curvy surface, a corner, or a coarse mesh you should see better performance and accuracy.

Webinar Files: Moisture Diffusion Modeling with ANSYS at R14 and Beyond

On May 24, 2012 Matt Sutton gave a well attended webinar on the new moisture diffusion modeling capabilities in ANSYS Mechanical APDL at R14.

image

Although we didn’t get a successful recording for this one (Matt has been chastised and done his penance for forgetting to turn on the recording…) we do have a PDF of the PowerPoint and a copy of the sample macro he used:

Coordinating Coordinate Systems in ANSYS Mechanical

Coordinate systems are one of those things that are fundamental to Finite Element Analysis, but that most of us do not think about a lot.  They are there, but some users never fiddle with them. And some users are constantly futzing around with them.  We thought it would be a good idea to do a quick review of how they work in ANSYS Mechanical.  We will also go over the basics for  Mechanical APDL (MADL) in case you need to work with snippets.

Why Coordinate Systems Matter

ANSYS cares a lot about coordinate systems because they allow the program to solve in a standard, global, Cartesian system while allowing loads, constraints, material directions, layer information, beam sections, joints, result values, and a whole slew of other important aspects of the model to be specified in unique coordinate systems. This avoids making the user do coordinate system transformations.  At solve time, everything gets converted.

Since everyone reading this is an engineer, I’m going to assume that everyone already knows what a coordinate system is.

Coordinate Systems in DesignModeler and CAD Tools

It is important to start at the beginning.  Design Modeler and all CAD packages I’m aware of allow you to define some sort of coordinate system. Usually just Cartesian.  In workbench you can import those coordinate systems into ANSYS Mechanical by clicking “Import Coordinate Systems” from the “Advanced Geometry Options” properties for the Geometry cell in you systems.

For DesignModeler, there is an extra step.  Even if you turn on the import properties you need to dell DM which coordinate systems you want imported.  But first, be aware that there is no “coordinate system” entity in DM.  Instead it has planes, which is a coordinate system where you draw on the Z-normal plane. 

To make these available in ANSYS Mechanical, you need to scroll down to the bottom of the details for the planes you want converted over to coordinate systems, and set “Export Coordinate System” to Yes.

The following three images show setting it in DM, setting the property on the Project page, and how it shows up in Mechanical:

image  image  image

Creating Coordinate Systems in ANSYS Mechanical

In ANSYS Mechanical, coordinate systems reside in the Model Tree between Geometry and Connections.  Once you define a coordinate system it becomes available for use with any other object that can use a coordinate system.  This allows you to define it once, and then use it many times.

You always get a Global Cartesian coordinate system, called Global Coordinate System.  It is Cartesian, has an ID of 0, and sits at 0,0,0.  You can not change any of these values. Any imported coordinate systems will show up underneath the global.

To create a coordinate system you Right Mouse Button (RMB) on the Coordinate Systems branch and Insert->Coordinate System.  Or, when you click on the branch you also get a Coordinate System toolbar:

image

Click on the three color triad icon and a new system will be inserted.

Let’s look at each of the options in the details view.  But note before you go there, that the first set of group define a starting location and orientation, then you apply transformations in the last detail group in order to modify those locations.

  • Definition Group: This group specifies the type and MAPDL number for the Coordinate System
    • Type:  You can have the default Cartesian or Cylindrical here. The resulting coordinate system triads show up on your model like so.  As you can see, Z is the rotational axis, Y is tangential an X is radial.
      image   image
    • Coordinate System: In my opinion this should say Coordinate System ID because this detail lets you decide if you want ANSYS Mechanical to assign the number that MAPDL will use, or if you will.  Program Controlled is the default and is fine in most cases.  If you need to wrote a snippet to work with a coordinate system then you should change it to “Manual” and Coordinate System ID will show up.  Set it to any number over 11.

      image

  • Origin Group:  This group defines where the center of the coordinate system is.
    • Define By:  You can specify a Geometry Selection or Global Coordinates. 
      • Geometry Selection: The cool thing about using Geometry Selection is that as you update your CAD model, the origin will shift with it.  As with any geometry specification, you click on a surface, line, vertex or a collection of these.  Mechanical will calculate the geometric center of the entity of entities that you picked and place the origin at that centroid.  It will also shows the position in the global coordinate system below your geometry selection, but you can not change them.
      • Global Coordinates: Here you simply put in an X, Y, and Z value in one of two ways. The easiest is to just type them in.  Or, you click “Click to Change” for Location and pick the coordinate picker image icon and move your mouse over your model.  Mechanical calculates the point under the cursor (surface closest to camera) and displays it. When you click it will create a little blue cross on the geometry.  Choose apply on Location an it will enter that point in as the origin.  Kind of cool, if a bit inaccurate…
        image
  • Principal Axis Group: You need to tell Mechanical how to orient the coordinate system. By default it will align with the global.  But you can use Axis and Define By to specify that any of the three axis are aligned with a global axis, or with a piece of geometry.  Aligning with geometry is very useful because this is how you get coordinate systems aligned with your geometry. And when your geometry updates, that coordinate system aligns with the updated geometry.  This is especially useful when specifying a coordinate system in a cylinder because you can pick the cylinder face for your Z axis and it will move with the cylinder.
    Note that you can not specify align with Global –Z. If you want to do that you need to align with Z and use the transformation below to flip that.
    One option for “Define By” is “Fixed Vector” This uses the current orientation but disassociates it from the geometry.
  • Orientation about Principal Axis Group:  One point and a vector does not a coordinate system define. You have to specify an orientation around that principal axis.  You do that just like the how you specify that principal axis.  Define a global X, Y, or Z or a piece of geometry.
  • Direction Vectors Group:  These show the vectors for X, Y, and Z.  You can’t change them (I wish you could) and they are not a parameter. But they are useful.
  • Transformations Group:  This area allows you to stack offsets, rotations, and mirrors.
    You use the Coordinate System Toolbar to insert transformations into this group.  They are executed in order from top to bottom and the resulting orientation and position are shown in Directional Vectors and Transformed Configuration.
    There is a “Move Transform Up” and “Move Transform Down” icon as well in the toolbar to move the transformations around. There is also a delete to remove one.
    Note: When you click on a transformation in the list, the coordinate system on your model is shown AT THAT STEP, not at the final position.  This always confuses me.  So make your change, then click on the last step to see it.

Using Coordinate Systems

This is the easiest part. You simply choose one of your defined coordinate systems from a dropdown list when you create an object that is dependent on a coordinate system.  Usually this is when you can define a value based Components rather than on geometry:

 

image

Do note that you can also use coordinate systems to transform directional result values.  Simply pick the Coordinate system from the dropdown list.  This is especially important when looking at hoop or radial stresses in a cylindrical part.

Coordinate Systems in ANSYS Mechanical APDL

Coordinate systems are huge in MAPDL.  Nodes have them, elements have them, sections have them. Plus you can make a coordinate system active and every command you execute is done in that active coordinate system, and converted for you to the global. Very powerful.

If you do a search in help on “Coordinate System” you get hundreds of hits in the MAPDL manual.  Way too much to go over here.  We do recommend that you start with:

Mechanical APDL // Modeling and Meshing Guide // 3. Coordinate Systems // 3.1. Global and Local Coordinate Systems

It explains the types, the math, and the commands needed.  Read that, then move on to 3.3, 3.4, and 3.5 which talk about nodal, element and result coordinate systems.

Some key things every user should know are:

  1. All coordinate systems are defined by a number.  0-10 are reserved by MAPDL for its use.  Users can do 11 or higher.
  2. MAPDL has 6 default coordinate systems:image
    0 = Cartesian
    1 is cylindrical down the Z axis
    2 is Spherical
    4 is Cartesian, same as 0
    5 is Cylindrical down the Y axis.
    6 is Cylindrical down the X axis (not shown)
    I have no idea what happened to 3 or why 4 is the same as 0.
  3. When you change the active coordinate system with CSYS, all commands that involve coordinates get transformed into that coordinate system.  So:
    local,11,1,2.5,0,0,0,90,90
    n,1,10,10,10
    Actually makes a node at 12.5,9.8481,1.7365 in the global coordinate system.
  4. You can show local coordinate system with /psymb,csys,1

    image

  5. You can list your coordinate system definitions with CSLIST:

    image

  6. Only Cartesian and cylindrical are supported in ANSYS Mechanical, so if you need to use spherical or Toroidal you need to use snippets

Thoughts

Make sure you understand how Mechanical is using coordinate systems by bringing your models up in MAPDL.  Look at your nodes and see if they are rotated and how.  Check the coordinate systems with a CSLIST. Make sure you feel comfortable, don’t take it for granted.