Error: FLOAT: invalid argument [1]: wrong type [not a number]
 

Hello guys,

I am getting the following error with ANSYS Fluent 14.5 x64 in Win7 Home Basic. Firstly, I searched the similar errors from this forum and also from google. I found a few responses, not a specific answer.

Some of them is relevant to re-mesh.
Somebody says close Fluent and re-open Fluent. (The ANSYS Support team response :confused:)

I tried the these responses. I have changed my mesh four or five times. I re-check my geometry and my mesh skewness. I closed and re-opened Fluent, too. I changed boundary conditions. I have changed some solution options. However, I couldnt figure out the solution for this error.

Last week, I got good calculations from similar geometry and same options in Fluent. Two weeks ago, I got the same error and I remeshed and solved the problem, but it doesnt work this time.

Now, I am getting this error. I am looking forward to your helpful responses.

-------------------------------------------------
Error: cx-xy-plot-data: invalid number
Error Object: 1.#inf

Error: cx-xy-plot-data: invalid number
Error Object: -1.#inf

Error: cx-xy-plot-data: invalid number
Error Object: 1.#inf
step flow-time Cm-1 Cl-1 Cd-1
1 3.0000e-02
Error: FLOAT: invalid argument [1]: wrong type [not a number]
Error Object: 1.#inf
----------------------------------------------------

haha.
Seems better to restart fluent.

Hi Saeed Sadeghi,

I want to also share my experience last night with same error. I checked the previous calculations which are same geometry but smaller domain and solved with 5000 iterations in transiet time. I maintained the calculation with 50 iterations. It didnt give any error, also calculated the drag, lift coefficients.

After this calculation, I duplicated the fluent in workbench and just changed the time to steady from transiet. I didnt changed anything, and it gave me the same error. Besides, it happens in another computer.

Please, any ideas....?

Error: FLOAT: invalid argument [1]: wrong type [not a number] SOLUTION
 

I had the exact same problem. You have set a moment coefficient monitor, which requires both a projected area, as well as a characteristic length, in the Reference Values options. My problem was that the characteristic length was set to zero. Make sure that both the characteristic length and project areas of your simulation are not zero. I'm assuming that you're simulating an external flow? Hope this helps.

Hi, brksnn,
I also came across this problem. I solve according the following idea. good luck
http://www.cfd-online.com/Forums/flu...-object-f.html

Hi to all. I have solved the same problem with the modification of the velocity Reference number that was set to 0. Since it is used in the lift/drag coefficient calculation, the division was by zero.

Solved it
 

As I read through comments and @bmahnic mentions the velocity in reference numbers, it solved for me.

In reference numbers although I checked ''From Inlet'' but velocity was zero.
I clicked on inlet again and it changed to my inlet velocity in boundary conditions.
:)

For me it was the monitors. I deleted and added again with print to console, and it worked for me. Hope this helps:)

Hi,I want to offer another solution method that might help.
Pls reopen Fluent using DOUBLE precision option.