ElectroMechanical Transducer Permittivity in ANSYS Mechanical

EM Transducer is a boundary condition commonly used in the simulations of MEMS devices.  Workbench users can download the Piezo & MEMS ACT module from the ANSYS Customer portal to gain access to EM transduce capabilities.  EM Transducer automatically generates TRANS126 elements in Workbench based on the EMTGEN APDL command.

The EM Transducer object uses permittivity of Air as a default and does not allow users to define their own permittivity.  If a user wants to define a custom permittivity, they can create an APDL command object that updates the 7th real constant of the generated TRANS126 elements.  See the sample code below:

 

 

!!! EXAMPLE APDL CODE  !!!
epsr=ARG1                                          ! USED TO DEFINE THE RELATIVE PERMITTIVITY
                                                               ! IN THE DETAILS OF THE COMMAND FILE
fini                                                         ! LEAVE THE SOLUTION PROCESSOR
/prep7
esel,s,ename,,126
*get,nelems,elem,,count                   ! nelems = NUMBER OF THESE ELEMENTS
elm=0                                                   ! INITIALIZE ELEMENT NUMBER
*do,i,1,nelems elm=elnext(elm)      ! elm = NEXT HIGHEST ELEMENT NUMBER
*get,rnum,elem,elm,attr,real           ! rnum = REAL CONSTANT ID # ASSIGNED TO ELEMENT elm
*get,r7,rcon,rnum,const,7                 ! r7 = VALUE OF 7th REAL CONSTANT IN REAL CONSTANT SET #rnum
r7_new=epsr*r7                                  ! MODIFIED VALUE TO SUBSTITUTE FOR ORIGINAL VALUE
rmod,rnum,7,r7_new                         ! MODIFY THE 7th REAL OF REAL CONSTANT SET ID #rnum
*enddo

 

fini                                                          ! LEAVE PREP7
/solu                                                       ! REENTER THE SOLUTION PROCESSOR
alls

Subscribe to Newsletter

  • This field is for validation purposes and should be left unchanged.

 


How to Parameterize Everything in ANSYS

kaan-80x80One of the best ways to get value out of your simulation is to do parametric analysis. With very little marginal work a completed model can be parameterized to simulate scenarios limited only by your computational time and resources (have you considered a Parametric Pack for parallel design solves?). With ANSYS R18’s promise of digital exploration, DesignXplorer is now included with all CFD, Mechanical and Multiphysics bundles. Sophisticated parametric exploration, optimization and robustness is now at your fingertips. While ANSYS Workbench and DesignXplorer manage your parameters in a consistent interface, setting up a parameter is different in each of the software tools and not always obvious. This document is intended to be a quick reference of how to do so, letting you get over this initial hurdle to take full advantage of the promise of Digital Exploration.

Table of Contents (for quick jumping around):

 

SpaceClaim Direct Modeler

SpaceClaim let’s you create a parameter from almost any operation:

Param - SpaceClaim Simple

Your parameters show up in the Groups tab.

For more advanced driving dimensions you need to have a dimension on an annotation plane:

Param - SpaceClaim Advanced

 

DesignModeler

DesignModeler has the familiar checkbox to “promote” parameters out to Workbench:

Param - DesignModelerYou can create relations between promoted parameters and other dimensions in the model with the Parameters Pane.

CAD Systems

With the appropriate associative interface licensed and configured, you can make Workbench aware of CAD parameters.

Param - CADBe sure to either use the DS or ANS prefix or else ANSYS will ignore your parameter. You can modify this with the Parameter Key property shown above.

Mechanical

In Mechanical, anywhere you see the checkbox can be promoted to a parameter for Workbench to use:

Param - MechanicalMechanical Command Snippets

APDL command snippets used in Mechanical can also be parameterized, both as input parameters:

Param - Mechanical APDL In

and output parameters (any variable with the Output Search Prefix will be retrieved):

Param - Mechanical APDL OutBe aware that APDL command snippets are not units aware!

Mechanical APDL (ANSYS Classic)

You can also easily use script files from the older user interface in Workbench, easily. With the Mechanical APDL component, specify the input file (along with supporting files as a reference file) and it will be parsed for all of it’s variables. All that’s left is to specify what’s an output and what’s an input:

Param - MAPDL

Fluent

In Fluent, most places that you can enter a value will have a dropdown that allows you to specify a parameter instead:

Param - Fluent

CFX-Pre

In CFX-Pre you can specify expressions as parameters and use them as inputs in other parts of the model:

Param - CFX

CFD-Post

In CFD-Post you base parameters off of expressions as well, making sure to use the nice right click menu to help with building expressions:

Param - CFD-Post

Maxwell & HFSS

The user interface is similar enough in these tools so that the same instructions apply. When accessing these from Workbench, a DesignXplorer node is created under the Optimetrics portion of the tree. Optimetrics is an EMAG specific optimization tool that is complimentary to DesignXplorer. In most places in Maxwell and HFSS, enter an identifier instead of a number to automatically create a parameter. Promote it out to Workbench in the DesignXplorer node. In the DesignXplorer node, output variables can be created in the Calculate tab.

Param - Maxwell HFSS

Icepak

Similar to the above, in the user interface where you would normally enter a number, instead enter an identifier preceded by $. Then in the Define Trials dialog, expose the parameter to Workbench.

Param - Icepak

And that’s it! Remember that the power of an integrating platform like Workbench allows you to have several of these software tools be connected in the same analysis flow. From CAD Parameter interaction to coupled field analysis, it’s all possible. Now go forth and digitally explore your design space!

Keep up to date on hardware and ANSYS simulation news and tips by subscribing to our newsletter:

 

Subscribe to Newsletter

  • This field is for validation purposes and should be left unchanged.

APDL Arrays & Tables Quickreference

Tech Tip: Bonding, Adhesion and Changing Contact Status In ANSYS Mechanical

kaan-80x80Did you know how easy it is to simulate thermal bonding in ANSYS Mechanical? You do not have to use our Element Birth/Death extension or deal with pinball regions. You can just raise the temperature of the body in a Static Structural analysis with a simple Thermal Condition. An example of this is below.

TBND Example

The secret to doing this is the TBND property, good ole real constant #35. If this seems like gibberish to you, this may be a good time to check out the Contact Technology Guide in the Mechanical APDL documentation or to check out the image below:

techtip_tbnd_apdl

Your contact in Mechanical already has a real constant that contains things like the normal contact stiffness (#3: FKN) and pinball region (#6: PINB) and all the other extra information that goes into contacts. If we want to add to this for a given contact, we can insert a command object and take advantage of the helpful cid and tid parameters that Mechanical provides. Taking advantage of TBND is as simple as using the appropriate APDL command to set real constant 35 to our critical bonding temperature of 30 (units in whatever you have selected at the time). We have to do this twice just in case the auto-symmetric algorithm switches the target and contact surface on us (make sure to review the Mechanical Nonlinearities Training if you don’t know what this means).

The once the temperature of the contact surface exceeds the TBND temperature, they are bonded forever. If you are feeling frisky, you can substitute an APDL table (or even a UPF) and have the bonded behavior depend on time, temperature, contact pressure or penetration. In this scenario, instead of setting a critical bonding temperature you would return 1 or greater to change to bonded, depending on the quantity that you choose. A nice way to simulate other types of adhesion!

You can download the project shown in the above animation below:

If this was useful to you and you’d like to hear more, subscribe to our newsletter below:

Subscribe to Newsletter

  • This field is for validation purposes and should be left unchanged.