Hints, Tips & FAQ
This page lists some suggestions that may help in a Zencrack analysis. Some items may be specific to particular Zencrack versions.
The page lists general issues - for issues specific to the finite element interfaces, please refer to the finite element interface support page.
What steps can I take to ensure that my cracked model is "correct"?
Firstly you should analyse the uncracked model before running a cracked model. Carry out the usual finite element checks. For example:
- are the support boundary conditions correct?
- if there are separate bodies coming into contact, does each have sufficient initial constraint (i.e. rigid body modes are correctly suppressed) ?
- are the load boundary conditions and resulting support reactions correct?
- is the stress distribution sensible?
- is the displaced plot sensible?
Once the uncracked mesh has been verified the initial cracked model can be analysed. These checks should then be repeated on the initial cracked model before undertaking a crack growth analysis.
Refer to the Getting Started Manual for more information.
How can I visualise the calculated crack growth profiles?
Use the Zencrack GUI - it allows direct import of analysis results and display of profiles. The results can be plotted to show the crack profiles and crack surfaces with controls on the rendering of point, line and surfaces.
As an alternative, the legacy utility program 3dmesh reads the .shp file from a growth analysis and generates a mesh consisting of beam elements to represent the growth profiles. The initial open part of the crack face is also represented. This mesh can be read into a pre-processor to visualise the crack growth. The 3dmesh utility is executed using "runzcrXX 3dmesh" from the folder containing the job files. Refer to the Utility Programs Manual for more information. Note that this method is now considered a legacy method and provides support only for the Abaqus and Ansys interfaces.
How can I generate a vs N data from the analysis results?
The Zencrack GUI is the best way to produce xy plots, including a vs N. Two types of xy data can be obtained:
- XY/FE data allows plotting of xy values at the "snapshot" positions at each finite element analysis.
- XY/BK data allows plotting of detailed results for one or more crack front nodes through the integration process.
For the most detailed integration information for one or more crack front nodes, use the *OUTPUT, TYPE=Integration option to request generation of additional output for one or more crack front nodes as the analysis runs. This information includes crack growth and cycle count as well as other data from the integration process. The output is generated in .bk files which can be used directly by the Zencrack GUI or via a spreadsheet program for plotting. This is called the XY/BK data.
The above method requires a request in the input file. If this is not done, or for an alternative way to plot results, the data in the .rep file can be used to produce plots in the Zencrack GUI using XY/FE data derived from the positions at which each crack profile was analysed during a growth run. The "process" utility program can also be run outside the GUI to generate a csv file for XY/FE results data that can be imported into a spreadsheet:
- one or more crack front nodes
- a parametric distance along each crack front
- at intersection of each crack front with a plane.
Because the data originates from the .rep file, it relates to "snapshots" at which the f.e. analyses occur during the integration process and hence is called XY/FE data. The GUI is the easiest way to access the XY/FE data but the "process" utility can be executed using "runzcrXX process". Refer to the Utility Programs Manual for more information.
The "da" data generated is obtained by summing the differences in nodal coordinates of a node from one crack profile to the next. Due to the shifting and re-distribution of nodes along a crack front during crack growth, this may produce misleading results for nodes on the "interior" of a crack front if the "node" method is selected. It is recommended that the node method is only used for surface node positions (and "deepest" node positions in symmetry models).
A discussion on the differences in these two methods (i.e. detailed integration data in XY/BK data vs fe snapshot data in XY/FE data) for plotting xy results can be found in the user manuals e.g.:
- v9.0 / v9.1 / v9.2 / v9.3 User Manual, section 8
- v7.9 / v8.0 / v8.1 / v8.2 / v8.3 User Manual, section 9
- v7.9 / v8.0 / v8.1 / v8.2 / v8.3 / v9.0 Examples Manual, examples ex04 and ex07
How can I create crack growth animations?
Animation options in finite element post-processors are geared towards producing animations from results in a single finite element results file. For crack growth animations showing the cracked meshes the requirement is to produce an animation by taking one snapshot from each of several results files.
In order to create such an animation the necessary results file must be saved for each finite element analysis of a crack growth run. This is done using keyword *SAVE with a request for the appropriate output file, e.g. ODB=YES, DB=YES, OP2=YES.
Each of the result files must then be post-processed in turn using the same viewpoint and scaling. Each of these images must be saved, e.g. to a .png file. The options for this depend upon the post-processor being used.
Animation of the crack growth profiles is supported directly
within the Zencrack GUI via the "Display crack profiles" screen which is
either via the Results screen or directly from the "Viewport
selection" screen. The crack profiles should first be displayed via the
"Viewport selection" screen.
When the "Display crack profiles" screen is opened it then
includes an "Animate" panel. This panel allows the active crack profiles
to be animated.
Each frame of the animation may optionally be saved to a .png
file. This type of animation may include a cracked or uncracked mesh
within the viewport.
If the *SAVE keyword is used to save the cracked meshes, it is also possible to load them one-by-one into the GUI to save a .png file for a given viewpoint. This enables creation of a sequence of undeformed mesh plots through a growth analysis. Crack growth profiles and/or surfaces may optionally be included on such plots.
What units should I use for my crack growth data?
Zencrack does not have any knowledge about the consistent units that are used for the finite element analysis. Therefore it is the user's responsibility to ensure that the crack growth data is in units that are consistent with the f.e. data. For example, if the f.e. model is defined with millimetre coordinates and MPa stress units, the crack growth data should be in terms of:
stress intensity factor : MPa mm0.5
da/dn : mm per cycle
The greatest scope for error lies in conversion of the Paris C constant (and equivalent term in similar laws). Depending upon the growth model being used, from Zencrack 7.8-1 the UNITS-K and UNITS-RATE options on *CRACK GROWTH DATA can be used to allow input of data in one unit system when the analysis is being carried out in another unit system. This removes the need for manual unit conversions.
If the units of the crack growth law are grossly incorrect, the analysis will either produce tiny or huge cycle counts, possibly resulting in the analysis stopping after the first f.e. step.
A unit conversion utility is supplied with the program documentation and is also available here to help with conversion of data between commonly used unit systems. Additional comments on unit conversions can be found in section 4 of the v7.9-2 / v7.9-3 / v8.x / v9.x (or section 3 of the v7.9-1) Getting Started Manual.
The rep file reports crack front nodes are "closed". In a displaced mesh plot the crack is open. Why?
This is probably due to the tolerance value of TOLOPEN. When considering the crack face opening displacements, Zencrack has a tolerance value below which a status of "closed" is defined. By default this is 0.0. Sometimes there can be a small amount of noise in "zero" values and small positive values really should mean "closed" (this is more the case for complex crack geometries than simple one-sided mode I problems).
To trap these small values, the TOLOPEN tolerance can be changed. There are two ways to do this:
- locally for the job - by adding a line to the zcr file as indicated in the warning below:
- globally for all analyses - by editing the value of TOLOPEN in the file "Zencrack folder"\defaults\tol.dat; this file contains defaults for a variety of tolerances. (For version 7.9-2 and earlier, this file is located in the \crack sub-folder).
If the value of TOLOPEN is changed, for example, to 1.0e-6 (by using *CONTROLS,TOLOPEN=1.0E-6), and "zero" displacements occur, a warning similar to this will appear in the rep file:
***WARNING There are 86 crack face nodal positions with opening displacement between 0 and the tolerance value TOLopen = 1.000000E-06. These nodes are treated as being closed. Please check that the value of TOLopen is appropriate for this analysis. TOLopen can be reset in the zcr file by using: *CONTROLS,TOLOPEN=value
The consequence of a "closed" crack front node is that a -ve sign is applied to the G and K values to indicate the closure. In a growth analysis there will be no growth for the node (an exception may be if there is a superposition load system). See section 3.3 of the v9.x User Manual or section 4.3 of the v7.9 / v8.x User Manual for further discussion.
Energy release rates have been processed but there are no stress intensity factors. Why?
The Young's modulus and Poisson ratio were not available to Zencrack. Ensure that the *MATERIAL keyword is used.
My cracked mesh has inside out elements. Why? [crack-block method]
If it is the initial cracked mesh:
- the initial crack may be too distorted e.g. large or small edge ratios for the crack-block or one large and one small edge ratio for the crack-block
- the uncracked element(s) may be too distorted
- you may have requested a combination of *MAPPING options that does not work well together.
If it is a cracked mesh part way into a growth analysis:
- the crack may have grown past the acceptable size limit in the crack-block and distortion is too great
- the crack front may have become too curved for the crack-blocks to handle resulting in inside-out elements inside the crack-blocks
- relaxation of the region surrounding the crack-blocks may not be able to remove excessive distortion outside the crack-blocks.
From version 7.8-3, if Zencrack identifies potentially inside-out elements when creating a cracked mesh, an element set ZCR_PROBLEMS is created in the cracked mesh input file. This can be post-processed to identify the location of the problem e.g. by importing the cracked mesh into the Zencrack GUI and highlighting/selecting the set ZCR_PROBLEMS in the VS screen.
How can I ensure that the crack region is loaded in the cracked model when I apply centrifugal load? [crack-block method]
For the Abaqus interface you need to define an element set that contains all the elements in the uncracked mesh and apply the load to that element set. When Zencrack generates the cracked mesh the element set is updated to include the new crack-block elements and so the load gets applied to the entire crack region.
For the Ansys and Simcenter Nastran interfaces there are no special requirements.
The boundary supports are missing from the crack region in my cracked model. Why? [crack-block method]
In Zencrack there are special requirements for the way that boundary conditions are specified on the elements that are replaced by crack-blocks. These requirements are stated for different finite element interfaces in sub-sections of section 2 of the Interface Manuals. Check that your uncracked mesh satisfies these requirements.