Viscosity as a function of Shear Rate?

[Anonymous]

I'm working on a new project involving plastic flowing through a channel.  The viscosity of the plastic changes as a function of shear rate and I'm not sure how I should be modelling this material.  Has anyone done this before?

[marco.mueller · Accepted solution]

Hi,

you have to create a new material where you specify a variation method for the viscosity and make the material variable (allow the viscosity to change), see attached images. Further information on the variation methods can be found here.

[Anonymous]

Thank you!  Very helpful and very quick response.  I will give that a try.

[Anonymous]

I'm having trouble with this fluid flowing through a serpentine pipe.  The outlet pressure is known and is set as a boundary condition.  The inlet pressure is also known but does not correspond to the simulated value.  The simulated pressure drop is approximately 75% lower than it should be.

Input variables I have used for this material are Density and Viscosity.  The material is highly viscous (per the PDF attached to the first post, above) and I have used the piecewise linear input method to input viscosity at 210 deg C. 

Three questions:

Is this the best way to model the material shown in the datasheet?

Is there a difference between Shear Rate and Strain Rate?

Are there other variables that would contribute to this gross error in pressure drop?

Thank you.

[marco.mueller]

Is this the best way to model the material shown in the datasheet?

It should be sufficient. If you have problems guessing the viscosity values from the datasheet points it may be helpful to use an automatic tool for this like this one. I'd double-check if the result strain rate is within the available data range. If not Simulation CFD will not extrapolate the values but instead use the nearest value from the table.

Is there a difference between Shear Rate and Strain Rate?

Not for this software.

Are there other variables that would contribute to this gross error in pressure drop?

Apart from the general ones like mesh and number of iterations (convergence), it may be helpful to try out the advection scheme ADV 4 that is designed for flows in long narrow pipes (if this is the case).

Do you specify a flow rate at the inlet?

It may be also helpful to move the inlet/outlet-faces away from regions of high gradients, to allow the flow to develop (inlet) and calm down (outlet).

Is the flow laminar or turbulent? If the latter it may be necessary to use the Low Re type of the kEpsilon turbulence model, since the boundary layer may be relativly thick. If this is the case (kEpsilon turbulence model not appropriate due to a thick boundary layer in relation to the mesh), it is usual that the pressure drop is under-predicted. See the corresponding help topic ( > Wall Model) for more information on this.