Defining an element surface for DFLUX with UEPACTIVATIONVOL? 1

[scooke]

Hello,

I am doing an additive manufacturing simulation in ABAQUS/CAE.

I have two working subroutines: DFLUX and UEPACTIVATIONVOL which both do their jobs correctly in separate models. I need to combine them but for my moving surface flux, the surface I define in the model does not work due to the activating elements during the analysis form the UEPACTIVATIONVOL. (The surface I define in the GUI for the heat flux does not exist at t = 0 since the elements are inactive)

Is there a way to define the top element face as a surface and change that in a subroutine for my DFLUX subroutine to call so the heat source will be applied on the surface of elements on one layer and then apply to the elements top face on the next layer?

Thanks in advance for your help!

 

[FEA way]

You can use the built-in features that were fairly recently added to Abaqus. For heating there is so called toolpath-mesh intersection module. Thanks to it you can define heat source path (position at each moment in time) and the software will take care of the rest. Elements close to the defined path will be heated. There's also a special feature for cooling of AM parts called progressive cooling. It applies convection and radiation conditions to all surfaces exposed to air (it accounts for changes due to activation of elements).

 

[scooke]

Thanks for your reply!

So right now I have the laser defined at the top of the wall as shown in the figure.

When I select user-defined heat flux where would I define the surface that it acts on? I have tried to use a substrate and define it on that surface but it just goes underneath my elements.

I am using python to define my laser position and when my elements are activated as CSV files and using the subroutine to read the CSV files and write them to variables.

Is the toolpath-mesh intersection module in Abaqus 2019? I am currently working in 2017 but will be upgrading to 2019 in a few days.

 

[FEA way]

I think that it would be really hard to achieve this effect without the toolpath-mesh intersection feature which is designed for such applications. It was available even earlier through Additive Manufacturing plug-in but in 2019 version it's already built-in.

 

[scooke]

Thanks for your help.

I will try the tool path-mesh when I get Abaqus 2019 version up and running.

Also when you mentioned a special feature for cooling of AM parts called progressive cooling. Does this use the subroutine UEPACTIVATIONFACET with *Progressive cooling in the input file?

Thanks again,

Shaun

 

[FEA way]

Abaqus automatically tracks evolving surfaces and applies convection/radiation to them when element activation is used. You just have to define *FILM and *RADIATE keywords. Subroutine UEPACTIVATIONFACET is only needed if you want to modify the exposed area to which cooling is applied.

 

[scooke]

Oh thats pretty great. Can a UFILM subroutine to apply a moving convection coefficient form the inert gas flow around the nozzle be used with the specification of *FILM ? Or would there be any interferences between the two film definitions?

Thanks again for your replies, I really appreciate it.

 

[FEA way]

FILM subroutine and *FILM keyword work together. If there are values specified in the film condition definition (film coefficient and sink temperature) they will be passed into the subroutine. Use *SFILM with type FNU to specify nonuniform film condition with magnitudes provided by FILM subroutine. There are some examples in the documentation.