Software > Zencrack > Support > F.E. interfaces > Ansys

Interface to Ansys - support issues

This page gives information on the interface to Ansys that may help in running jobs and improving the performance you obtain with this interface. Some key items that you may have missed in the user manual are also included.

Which versions of Ansys is Zencrack interfaced to?

Zencrack is interfaced to Ansys/Mechanical APDL. Testing has been conducted up to and including Ansys 2019R1.

Using multiple CPUs for Ansys jobs executed by Zencrack

For Zencrack 7.7 to 8.3 there are two ways that the number of processors for Abaqus jobs executed by Zencrack can be specified:

  • Variable ZCR_OPTIONS_ANSYS in the zencrack.ini file (or OPTIONS_ANSYS for 7.7 and 7.8 in the runzcr script file) can be used to define parameters passed to the Ansys command line for all Zencrack jobs. The -np option can be added to this parameter. Refer to the file itself (located in the Zencrack tools folder) or the Installation And Execution Manual for more information about this variable.
  • The command line option "-fe" can be used when executing a Zencrack job. This defines parameters to be passed to the Ansys command line for that particular Zencrack job. The parameters should be surrounded by quotes. For example, to use 4 processors:
    runzcr83 -j jobname -fe "-np 4"
If the -np parameter is defined using both methods, the command line value takes precedence.

Note that from version 7.9-3 the Zencrack setup program requests information about the number of processors and configures the zencrack.ini file accordingly during the installation process.

Calculating j-integrals with Ansys

The Ansys j-integral capability was added via the CINT option in Ansys 11.0. Interfacing to this capability is available from Zencrack version 7.5 and requires the service pack release Ansys 11.0SP1 (or later).

Calculating j-integrals with pressure load in the cracked region applied using SURF154 elements

When including pressure load on the surfaces of brick elements, Ansys Workbench generates the load via SURF154 elements. Such surfaces are updated if they are on target crack-block elements (from Zencrack 7.7-2). However, contour integral evaluation in Ansys (up to at least v2019R1) does not support surface load applied via SURF154 elements. This leads to incorrect contour integral evaluation for any crack front node connected to a surface with pressure applied in this way. Since Zencrack only updates the surface without regard for the way in which that surface is used, this can cause incorrect contour integral evaluation without any warning being generated in the Zencrack .rep file. Note that Ansys will generate warnings in the .err and .out files that surface elements are not supported in contour integral evaluation, but will still carry out the contour integral evaluation and report potentially invalid results. Details of the warnings depend on the Ansys version. For example:

Version 14.5, 15.x, 16.x, 17.x, 18.x, 19.x, 2019.x:

*** WARNING ***                         CP =       1.342   TIME= 15:07:29
Fracture parameter calculation issue: Contour integration for crack 1   
includes surface elements which are not supported.  These elements are  
ignored, and the contour integration results may not be correctly       

Version 12.1 gives the second of the following warning types only, versions 13.0, 14.0 give both the following warning types:

*** WARNING ***                        CP =       0.796   TIME= 12:31:13
Error with CINT calculation: crack tip node attached to element type
that is not supported, Crack 1, crack tip node 549, element type 154.
Element will be ignored.                                             

*** WARNING ***                        CP =       1.061   TIME= 12:31:14
Contour integration for crack 1 includes surface elements which are not
supported.  These elements are ignored, and the contour integration    
results may not be correctly calculated.                               

As a workaround for this contour integral limitation there are two approaches:

  • Allow the calculation of the contour integrals but do not use them for driving the analysis. Displacement based results can be used instead via: *ENERGY RELEASE RATE, PREDICTION=DISPLACEMENT
  • Modify the uncracked mesh:
    • replace the SURF154 elements on the crack-blocks by TSHAP surface, and,
    • change the load application to direct load onto the target crack-blocks elements via SFE

Using Ansys solid model mesh commands

If an uncracked mesh uses geometry definitions and volume meshing (e.g. VMESH), it is possible that different versions of Ansys will produce slight differences in the resulting mesh e.g. different numbers of nodes and elements. Whether or not this will happen depends on the particular volumes being meshed and the Ansys versions.

In the context of a Zencrack analysis this has the implication that a valid Zencrack analysis which references a solid model uncracked mesh for one version of Ansys may generate errors in another version of Ansys because the underlying mesh is different (even though the uncracked model file is identical). The errors occur because the elements and node numbers used for crack-block definition are no longer valid in the "different" uncracked mesh that Ansys has generated. This is only a potential issue if:

  • There is need to change Ansys versions part way through a project, or,
  • A model is re-visited at a later date and re-run in a later version of Ansys.
As a workaround if this issue arises, it would be necessary to extract node and element definitions from the original uncracked model and create a new mesh-based uncracked model for use with the later version of Ansys.

Using Zencrack 8.3-1 (or earlier) with Ansys 2019 - change in Ansys version naming

In moving from Ansys 19.2 to Ansys 2019R1 the internal version number reported by Ansys has changed from 19.2 to 19.3. The Zencrack setup program for Zencrack 8.3-1 (and earlier) refers to version 2019R1 as version 19.3. The entry for ZCR_ANSYS_VER in the Zencrack .ini file should be 19.3 and the version reported in the .rep file will also be 19.3.

Using Zencrack 8.3-1 (or earlier) with Ansys 2019 - change in temperature extraction

The issue described in this section is due to a changed Ansys behaviour related to the OUTRES option. From the Ansys 2019R1 release notes:

"... the following command sequence behaves differently:


Prior to this release, this input would have also (potentially) written the following records to the results file: volume/energy, temperatures, contact data, nonlinear data, surface stresses, back stresses, current densities, electromagnetic forces, and heat generation rate. In this release, none of those values are written unless explicitly requested."

When Zencrack processes the results of an Ansys model, the nodal temperatures at the crack front nodes are extracted via a request for element-based temperatures (using *VGET with BFE, TEMP).

A request for element stresses via "OUTRES,STRS,ALL" in Ansys 19.2 or earlier would also have generated temperatures. Zencrack would correctly extract temperatures at the crack front nodes.

The meaning of the above change is that the request for element stresses via "OUTRES,STRS,ALL" in Ansys 2019R1 or later does not generate temperatures - a specific "OUTRES,ETMP,ALL" request is needed. If there are no temperatures available from the output requests the Ansys 2019R1 .out file will report that "The requested BFE data is not available". Zencrack will report all crack front temperatures as zero and calculate temperature dependent data from temperatures that are all zero.

For Ansys 2019R1 it is therefore necessary to ensure that an element temperature request exists in the uncracked mesh, whereas in earlier Ansys versions it was not necessary to explicitly request temperatures (as long as stresses were requested).

Using Zencrack 8.0-1 (or earlier) with Ansys 18.0

The issue described in this section is resolved in Zencrack 8.1-1.

When Zencrack processes an Ansys model there may be a requirement to run a "pre-pass" analysis with Ansys to extract information in a standardised format. Due to a change in the format of data written by the Ansys NWRITE command in version 18.0, Zencrack does not correctly process the output with the result that the analysis or read of a mesh into the GUI will fail.

For Zencrack versions up to and including 8.0-1 it is recommended to use Ansys versions up to and including 17.2 for full compatibility.

Using Zencrack 7.6 (or earlier) with Ansys 13.0 (or later)

Ansys version 13 was released after Zencrack 7.6. Some changes in Ansys 13 mean that Zencrack 7.6 cannot be used with Ansys 13 (or later) on Windows machines. If Ansys 13 (or later) must be used on Windows machines, it is necessary to use Zencrack 7.7 (or later). There are also limitations on Linux machines if Zencrack 7.6 is used with Ansys 13 (or later). The reasons for the incompatibilities with version 7.6 and Ansys 13, along with the errors that can occur, are outlined below.

Errors executing Ansys (Windows only)

The Zencrack 7.6 setup configures Ansys to run an executable called ansys.exe. For example in the runzcr76.bat file:

set ZCRANSYS="C:\Program#Files\ANSYS#Inc\v130\ansys\bin\winx64\ansys.exe"

Using this Ansys executable in Ansys 13 (and later) gives an error which Ansys reports in a dialog box on the screen:

The program can't start because AnsMPI.dll is missing from your
computer. Try reinstalling the program to fix this problem.

The solution implemented in the version 7.7 setup program is to refer to a version specific executable in the runzcr .bat file. For example, ansys130.exe:

set ZCRANSYS="C:\Program#Files\ANSYS#Inc\v130\ansys\bin\winx64\ansys130.exe"

However, if this change is made manually in a Zencrack 7.6 installation with Ansys 13 (or later), a further error occurs. This is because the command line arguments being passed from Zencrack 7.6 to Ansys that were valid for the v12 ansys.exe are not valid for v13 ansys130.exe:

Invalid I/O redirection, please specify -i inputfile -o outputfile.

There is no workaround for this problem with the release version of Zencrack 7.6. So the Windows version of Zencrack 7.6 can only be used up to and including Ansys 12.

Invalid j-integral results (Linux only)

A change was made to j-integral output in Ansys 13 - the sign of all j-integral output was reversed compared to results obtained in earlier Ansys releases. So even though the Linux version of Zencrack 7.6 can execute Ansys 13, the resulting j-integral values are returned to Zencrack with an incorrect sign. In a crack growth analysis this will result in a message in the .rep file that there is no crack growth after the first finite element analysis.

The displacement based results (using *ENERGY RELEASE RATE, PREDICTION=DISPLACEMENT) are not affected by this issue.

Although displacement based results can be used, it is recommended that Zencrack 7.7 be used with Ansys 13 (or later) to prevent this issue from arising.

Crack-block restrictions for Ansys 13.0 (or earlier)

Ansys historically had restrictions on the way that 8 and 20 noded elements can be degenerated - only certain collapsed patterns being allowed. In Ansys 14.0 these restrictions were removed. The prevention of the use of certain crack-blocks with Ansys which existed up to Zencrack version 7.8-2 is removed in version 7.8-3 if Ansys version 14.0 or later is being used (i.e. from Zencrack 7.8-3 onwards, it is possible to use all crack-blocks provided that Ansys 14.0 or later is being used). The previous restrictions on some crack-blocks still apply in version 7.8-3 if using Ansys 13 (or earlier). An attempt to use a crack-block which is not permitted will result in an error in the .rep file.

The crack-blocks containing collapsed elements that have restrictions are:

Crack-block(s) Zencrack version(s) in which restrictions apply
s02_q38x2 7.4, 7.4a, 7.5, 7.6, 7.7, 7.8-1, 7.8-2, 7.8-3 (and later)*
s03_q46x2 7.4, 7.4a, 7.5, 7.6, 7.7, 7.8-1, 7.8-2, 7.8-3 (and later)*
s04_q70x2 7.4, 7.4a, 7.5, 7.6, 7.7, 7.8-1, 7.8-2, 7.8-3 (and later)*
s05_q24x2 7.5, 7.6, 7.7, 7.8-1, 7.8-2, 7.8-3 (and later)*
sq38x2 7.1, 7.2, 7.3

* restriction only applies for Ansys 13 or earlier


Ansys and its logo are trademarks of SAS IP, Inc., a wholly owned subsidiary of Ansys Inc., Canonsburg, Pennsylvania, U.S.A.
Zentech International Limited is a member of the Ansys Preferred Solution Partner program.
Web link

Click here to visit the Ansys website
Previous item for this topic Abaqus/CAE plug-in F.E. interfaces
Simcenter Nastran Next item for this topic