In this blog, we will talk about units in Abaqus. Generally, Abaqus does not have inheritance unit system. On the one hand, I can be brief: we can do whatever we want if it is consistent. On the other hand, it is a frequent cause of errors. Hence, we will take a deep dive into unit systems.
Consistent units
As previously said, Abaqus requires that user must manage units consistently. It makes all difference based on which units you use. It is a good practice that allows the user to have a lot of flexibility. It is also prone to make mistakes, especially since user can’t specify which units were chosen anywhere. Most people use the same unit system all the time and assume that everyone else does as well. At least, that is what I do.
This can result in an intriguing circumstance, in which user duplicates a piece of material data from a colleague and obtain unanticipated consequences in the result. I have experienced this in the past, and it took me a while to realize he was using SI units in meters whereas I was using SI units with mm.
Bottom line: be aware that this may occur, check whether the values the user is putting make sense in the unit system being used and be consistent with the units in the model description.
Angles and rotations
Abaqus’ only built-in units are for angles and rotation. Abaqus measures rotational degrees of freedom in radians, while all other angles are measured in degrees.
Specifying physical constants
Many physical constants cannot be predefined in software because they may depend on the set of units used, which is an intriguing side effect of not using an inherent set of units. For example, when using SI with mm, the gravitational constant of 9.81 m/s2 becomes 9810 mm/s2 or 386 inch/s2 when the user uses different unit system. We must tell Abaqus the values of the physical constants used in the analysis because it does not know which unit system we are using.
For best example, consider gravity loading by defining the acceleration due to gravity (g), while applying a gravitational load. For another example, absolute zero temperature and the Stefan-Boltzmann constant must be supplied when surface emissivity and radiation conditions are specified in heat transfer analysis.
For majority of thermal analysis, If the universal gas constant is needed, it must be specified as well. User can provide that through model attributes, which can be accessed through model by clicking right mouse button à edit attributes.
Consistent Unit Systems in SI and US Standard
The following table can be found in the Abaqus manual:
Each column corresponds to a set of consistent units. So, for example, if we are using mm, N and s, we should also use mJ. It is highly advisable that a new user to Abaqus should refer this table prior to making input to their models.
It is always nice to know what order of magnitude is expected for different properties. In the table below, some examples of properties and physical constants are provided.
| Commonly used unit | SI value | SI-mm value | Multiplication factor from commonly used to SI-mm | |
| Stiffness of steel | 210 GPa | 210∙109 Pa | 210000 MPa | 1000 |
| Density of steel | 7850 kg/m3 | 7.85∙10-9 tone/mm3 | 10-12 | |
| Gravitational constant | 9.81 m/s2 | 9810 mm/s2 | 1000 | |
| Pressure | 1 bar | 105 Pa | 0.1 MPa | 10-1 |
| Absolute zero temperature | -273.15 ÌŠC | 0 K | ÌŠC and K both acceptable | – |
| Stefan-Boltzmann constant | 5.67∙10-8 W∙m-2∙K-4 | 5.67∙10-11 mW∙mm-2∙K-4 | 0.001 | |
| Universal gas constant | 8.31 J∙K-1∙mol-1 | 8.31∙103 mJ∙K-1∙mol-1 | 1000 | |
Considering the scenario in India, usually ̊C or K are used for temperature. The only difference between these units is an offset; a difference in temperature of 1 ̊C is equal to a temperature difference of 1 K. Because of this, ̊C and K can be interchanged in derived units: mW∙mm-2∙K-4 equals mW∙mm-2∙ ̊C -4.
Changing units in an Abaqus model
In some cases, user may want to change the system of units used. This can be done for varied reasons such as personal preference, to be consistent with units used by colleagues or because the original set of units leads to values that are so small or so large that numerical issues arise.
Unfortunately, there is no button to click in Abaqus to do a conversion: user will need to do this manually. This means going through all values specified and figuring out what they should be in the new system of units. If the user needs to do this often, it may be worthwhile to write a script for it.
If the unit of length is changed, this means that the part must be scaled. If drawn in Abaqus, the dimensions can be changed to account for the unit change. If the part is imported, this is not possible. The best possibility is then to copy the part while scaling it.
Because this leads to a new part, any loads and boundary conditions defined on the original part need to be redefined. Such a copy-with-scale should thus be performed before setting up the model. Furthermore, sets are not kept when copying a part this way. A workaround is to create a mesh part (in mesh module: mesh à create mesh part) and copying this. Sets are kept then.
If we are importing an orphan mesh where the scaling is not possible in which the dimension for the model is derived from the material properties defined. For example, if it is a steel part and we provide young’s modulus as 2.10 e9 then the units are considered as mm. Alternatively, we can change the system of units by altering the material properties, but the user must make sure that every unit are consistent.
Final remarks
Though using the correct units in general is not difficult, it is something to pay attention to. It is a bit like simulating half of a symmetric model: it is not that difficult to multiply forces by two to get the total force, but it is easily forgotten.
Leave a Reply