Get notified!

Automatically receive blogupdates from our FEA Experts about Abaqus and FEA

Simuleon FEA Blog

Units in Abaqus

Posted by Christine Obbink-Huizer on Feb 25, 2019 10:16:00 AM

In this blog, I want to discuss units in Abaqus. On one hand, I can be short on it: we can choose what we like, as long as it is consistent. On the other hand, this is a common source of mistakes. Therefore I want to go into a bit more detail.

Consistent units

As I said, Abaqus assumes you use consistent units. It does not matter which units you use, as long as they match with each other. (The only exception to this is below.) This is a nice approach allowing a lot of flexibility. It is also prone to errors, especially because you do not need to fill in which units were chosen somewhere. Most people use the same system of units all the time, and kind of assume other people are using the same units. At least that is what I do…

This can lead to the interesting situation where you copy a material from a colleague, and get unexpected results. I’ve actually done this, and it took quite some time to realize he was using SI units, while I was using SI units with mm.

Bottom line: be aware that this kind of thing may happen, check whether the values you have make sense in the system of units you are using and perhaps mention the units you are using in the model description.

                           

Angles and rotations

The only built-in units Abaqus has, are for angles and rotation. Abaqus uses radians for rotational degrees of freedom, while all other angles measures are expressed in degrees.

 

Specifying physical constants

An interesting consequence of not using an inherent set of units is that many physical constants cannot be predefined in the software because they depend on the set of units used. For example, the gravitational constant of 9.81 m/s2 becomes 9810 mm/s2 when using SI with mm or 386 inch/s2 when using US units. Because Abaqus does not know which unit system we are using, we must tell Abaqus the value of the physical constants that are used in the analysis.

For gravitational loading, this is done by specifying the acceleration when applying a gravitational load. When surface emissivity and radiation conditions in heat transfer analyses are specified, the absolute zero temperature and the Stefan-Boltzmann constant must be given. If the universal gas constant is needed, it must also be specified. They can be specified as model attributes, accessible via model --> edit attributes.

0_model attributes_Abaqus_units

 

Example

In the Abaqus manual, we can find the following table:

1_table_abaqus_units

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 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 tonne/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  ̊C

0 K

  ̊C 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

Here in the Netherlands, 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 different 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, you may want to change the system of units used. This can be done for different 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: you will need to do this yourself. This means going through all values specified, and determining what they should be in the new system of units. If you need to do this often, it may be worth while to write a script for it.

If the unit of length is changed, this means that the part must be scaled. If it is drawn in Abaqus, the dimensions can be modified to take into account the unit change. If the part is imported, this is not possible. The best option is then to copy the part, while scaling it.

3_scale part

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 retained when copying a part this way. A workaround is to create a mesh part (in mesh module: mesh --> create mesh part) and copying this. Sets are retained then.

 

Final remarks

Though using the correct units in general is not difficult, it is definitely something to pay attention to. It’s a bit similar to simulating half of a symmetric model: it’s not that difficult to multiply forces by two to get the total force, but it’s easily forgotten.

Need assistance for your FEA challenge? Request consulting

Topics: Abaqus, units

About our FEA Blog:

Simuleon blog topics related to Finite Element Analysis like; Structural Analysis and CFD analysis performed with SIMULIA Abaqus FEA, XFlow CFD, Isight Simulation Automation, Tosca Topology Optimization and Fe-Safe accurate Fatigue.

Subscribe to our Blog.

Search All Blogs

      Recent Posts

      Most Popular Posts

      Read All Blogs

      View All