[Michael104]

Hey everyone,
i am trying to calculate the heat production of a fuel cell and have some question. Therefore i want to use the PEMFC addon and plot the temperature of a single channel pem-fuel cell. I am using fluent 2019 R3.


**Question:**
When I run the case the the current decreases for anode and cathode from higher values to 0 A/cm². Also the the V-Open deceases from ~1.2 V to lower values like 0.8 V. After 20 Iterations i received the error floating point (see picture below). Does anyone knows what i am doing wrong?? I tried allot but nothing helps.
Thanks for any Help.


Settings:
- I created a single fuel channel without cooling, with mpl, cat, gdl,(fluid) ; mem & current collector (solid), with hex-mesh, 0.5mm x 0.5 mm x 30 mm channel with 101920 elements.


-I imported the geometry into ansys fluent and uses most of the default pemfc-addon settings,set under relaxation factors in PEMFc gui panel to disv´d-vap/liq. source to 0.01 and osmotic drag source to 0.5. Solution controls under relaxation factors to 0.3 for pressure and 0.3 for momentum, all other set to 1, operating pressure 200000 pa, temperature to 343 K and mass flow inlet anode to 3e-6 kg/s and cathode to 0.00011 kg/s. Wall terminal anode is set to 0 V and cathode to 0.3 V. Like it is said in the" Ansys fluent best practice document" I run the first 25 iterations without Joule heating and reaction heating, after these first iterations with most of the model options ( except anisotropic E-Cond. and Liquid Phase).



**Question:**
When I run the case the the current decreases for anode and cathode from higher values to 0 A/cm². Also the the V-Open deceases from ~1.2 V to lower values like 0.8 V. After 20 Iterations i received the error floating point (see picture below). Does anyone knows what i am doing wrong?? I tried allot but nothing helps.
Thanks for any Help.

Michael

[xq712000]

Hello, how did you solve the problem?

[xq712000]

Originally Posted by xq712000

Hello, how did you solve the problem?

Problem resolved by setting 'Cell Zone Conditions' of 'membrane' to 'fluid' rather than 'solid'

[xq712000]

Originally Posted by xq712000

Problem resolved by setting 'Cell Zone Conditions' of 'membrane' to 'fluid' rather than 'solid'

This is to ensure that the interfaces between membrane and catalyst layers are identified as 'Internal' boundaries

[xq712000]

Originally Posted by xq712000

This is to ensure that the interfaces between membrane and catalyst layers are identified as 'Internal' boundaries

Another problem to notice is that you have make sure the solid-fluid-interfaces are convert to shadow pairs (coupled-wall-BC) using different meshing tools such as Pointwise