Abaqus And The Command Window - Launch Jobs, Monitor Jobs, And More
Many Abaqus users will be familiar with the GUI that comes with most packages, Abaqus CAE, but have you ever wanted a little more customization when running your Abaqus jobs? This post focuses on running Abaqus jobs from the command window, and takes a look at some of the lesser known commands that might just help you in your next simulation!
The Abaqus Command Window is a powerful tool that allows users to perform advanced simulations, automate repetitive tasks, and customize the behavior of Abaqus simulations. Outlined in this post are some of the most useful commands that you can use in the Abaqus Command Window.
Firstly, we’ll need to have generated an Abaqus input file. This can be done in most pre-processors on the market, or if you’re an advanced user, even by hand. We’ll leave that for another post, but let’s assume that our input deck is named Job.inp.
Next, we’ll need to open the Abaqus command window. Check out the image below to see how to do this in Windows 11. It’s essentially the same for any version of Windows, although it might look a little different…
At this point we’ll need to navigate to the scratch directory, which is C:\temp as default. To navigate between folders in command:
'cd..' to move back a directory
'cd <DirectoryName>' or '<DirectoryPath>' to move into that particular directory
e.g. if you start off in C:\, type ‘cd temp’ to open the temp directory
Now that we have a window open and a job that we want to perform operations on, lets take a look at some of the more basic commands that are available when running jobs.
Job management commands include:
Job: The job command allows us to launch a new simulation. In our case we’d simply type ‘abaqus job=Job’ and Abaqus will begin to run our simulation
Datacheck: Adding the word ‘datacheck’ allows us to run a quick check of our input deck for any errors or issues that would come up in the .dat file during abaqus pre.exe. Using this lets us ensure that we don’t have any serious problems with the model prior to launching the main simulation
CPUs and GPUs: At the end of the line, we can define the number of cpus and gpus that we’d like to commit to the simulation. For example ‘cpus=4 gpus=1’ submits the job on four cores and one gpu
Interactive: Adding the word ‘interactive’ at the end of the line allows us to view the log (.log) file interactively as it’s being written. This can be particularly useful when we’re debugging jobs on the go
Suspend, Resume and Terminate: Finally, ‘suspend’, ‘resume’ and ‘terminate’ can be used to stop, start and kill your Abaqus jobs, respectively
Over the years, you tend to pick up on some of the more useful ‘power user’ commands that can really make your Abaqus workflows more effective and efficient. Here is a list of our favorite lesser-known commands that might just save your day!
Abaqus Version: When we’re running Abaqus, it might be necessary to revert to prior versions that are available on the computer that you’re running on. To do this, instead of simply typing ‘abaqus’, we’ll be specific about the version. Typically this will look something like ‘abq2017’ for the 2017 version, but that might change a little depending on the information in the environment (.env) file
Restart: If we want to use results from the end of a previous analysis at the start of our next one, after we’ve defined the new job, we need to let Abaqus know what the original job name was. To do this, after ‘job=Job’ we’ll type ‘oldjob=<OldJobName>’. This can be super valuable when we have a bolt preload step, for example. We don’t want to run that same step every time for each load case, so, instead, we use the results from the bolt preload job as the starting point for all of our future analyses
Double Precision: When running Abaqus/Explicit, it is often necessary to utilize double precision; especially when the number of expected increments gets very large. To do this, simply include the word ‘double’ at the end of your job submission line
Opening Files: It is possible to open ODB files directly from the command window. This can be useful if you’ve just run an analysis and would like to check out the results. To open viewer and view our Job, type ‘abaqus viewer odb=Job’
Running Python Scripts: Python allows us to do all different types of things with Abaqus, and running one from the command line couldn’t be simpler. Type ‘abauqs python <ScriptName.py’. If the script requires the kernal, but you don’t want to actually open CAE, type ‘abaqus cae noGUI=<ScriptName.py’
Launch Subroutine With Job: FORTRAN subroutines offer almost endless customization potential to Abaqus, but how do we run them once they’re complete? Easy! Add the ‘user=SubroutineName.for’ at the end of the command!
Unconnected Regions: And we saved the best (in our opinion) to last! Ever have a model that is failing because of rigid body motion, but you can’t figure out exactly which parts are the issue? This is for you. If you use the datacheck function described above and add in the term ‘unconnected_regions=yes’ at the end of the command, Abaqus will create a set/sets to let you know which parts in the model are not connected together. This can instantly let you know whether you just have a rogue part or there are a bunch of regions in the model that are not seeing each other. As you can imagine, that really helps save time when debugging big models!
And just in case that wasn’t enough:
Fetch Files: There is an oft-forgotten tool that would help many Abaqus analysts, and especially beginners, and we feel obliged to call attention to. When you install Abaqus, there are a number of example models that come with it. To ‘fetch’ them, type in ‘abaqus fetch job <JobName>’ and all the requisite files will be copied into the directory from which the command was run. To learn more about the files available, check out your documentation for Abaqus Example Problems, Abaqus Benchmarks and Abaqus Verification.
Hopefully, this post has provided a good Abaqus Command Window commands that can help you get the most out of your Abaqus software. Whether you are automating tasks, visualizing results, or debugging simulations, these commands can help you work more efficiently and effectively with Abaqus.
As we’re sure you’re aware by now, we’re here to help! If you would like to learn more about Abaqus, or even just pick our brains on something, don’t hesitate to get in touch with our team!