Scalar Parameter values dont get modified?

[imse]

Hi,

(using GUI method)

I have been trying to use scalar parameter to assign values to variables that I use in modeling the problem.. the first time I run the program it is fine, but when i modify these scalar parameters and re-run the program again, it computes result using the first set of parameter values

could someone tell me what I am doing wrong?

thanx
Robin

 

[Drej]

Your post is quite vague, and it's difficult to be accurate here since there's no knowing the processes you've carried out before/after this assignment. Explain a bit more about what you've done. Are you resuming the database after you have re-defined your parameters? This might explain why you are seeing this behaviour.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[imse]

Drej,

First - element type is selected, material properties are assigned and the object is modeled and meshed

Then using the scalar parameters, I assign values
eg: Covection_left=10, initial_temp = 25, heat_flux = 1e6,time_step=1.... I then add the boundary condition(convection), load (heat flux),transient time etc using the scalar parameter "names". Now when i solve this for the first time, it works.

After this when I start a new analysis, i modify the some of the scalar parameters,eg: heat_flux = 1e7 (instead of 1e6). and then try re-solving the problem, it gives me a solution based on the first set of scalar parameters (in this case, for heat_flux=1e6)

is there something else i should be doing?

thank you

Robin

 

[Stringmaker]

Robin,
What's making you think that the scalar parameters are not updating? Do you have any actual evidence of this? Or does your temperature distribution look identical between the two cases?
Is it possible that the heat flux is so large in both cases that the results each scenario yields turn out to be almost identical? You heat flux seems rather large for english or SI units. Just a thought...

Good luck,
-Brian

 

[Drej]

In theory there should be no problem with what you've done. As a check, I would write a little bit of code by hand to see if ANSYS is doing anything silly. Put the following into a text file in your working directory and read into your model (just to check the heat_flux parameter) using:

File>Read input from...

fini
/solu
alls
heat_flux=1e7
/output,check_heat_flux,out
*stat
/out
parsav,SCALAR,check_heat_flux_again,out

This should firstly output a text file called check_heat_flux.out, which will contain all of your parameters at the time of solution. Check to see if heat_flux=1e7. It also writes all of your scalar parameters to another text file called check_heat_flux_again.out (using the PARSAV command), so check in here to see if the heat_flux=1e7. If heat_flux=1e7 in both files, try and solve and see if ANSYS uses this value. If not we'll try something else...


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[imse]

To answer Brian's question... if i was not to use the scalar parameter and do the modeling using 1e6 heat flux, it would give me a temperature distribution range of 76 to 419 degrees, while 1e7 gives 535 to 3953degrees. (I'm try to model submereged arc welding process)

Drej,
by inputing the file that had your command lines, the output file data reflected the current scalar parameter values, but the temperature distribution result was for the initial scalar parameter
(i tried both ways, modelling with initial scalar parameter of 1e6 heat flux and latter changing it to 1e7, both results reflected 1e6's output temperture distribution and modelling with initial 1e7 heat flux and latter changing it to 1e6, reflected 1e7's output temperature distribution.)

thanx

Robin

 

[Drej]

Hmmm... You mention doing a transient analysis and then finishing and starting a new analysis, but how are you applying the heat flux? In fact, what exactly do you do (as a summary) in the GUI from start to finish for the two analyses?


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[meshparts]

Hi!

I have a silly question to Robin: Are you aware, that solid model and finite element properties are not automatically updated, if you just change the variables? I apologise to you, if my question is to simple. Just checking.

Regards,
Alex

 

[imse]

Alex,

no I am not aware of that.. could you please advice on this

Thanx

Robin

 

[imse]

drej,

the last couple of times that I was solving the problem, i was using steady state analysis - as it was easier to see if the effects of scalar parameter changes

Summary the modeling
There is a block with dimension .25m x.075m x.00945m... additionally, several smaller blocks with dimension: .0063m x.00315m x.001m are overlapping with the bigger block along one of the edges... heat flux is applied to one of face's of the smaller block...
If it were a transient analysis, first step: a heat flux is applied to the face of the first smaller block.. then i the next step, it is deleted from that face and then applied to one of the faces of the next smaller block... and so on till the last... basically an imitation of the discretized moving heat source in during a welding process..

thanx a lot

Robin

 

[meshparts]

Hi Robin,

Let's take an example. You want to define the density of your block through a parameter named "density".

You write:

density=7800

Then you assign define the material:

mp,dens,1,density

Even if you later redefine the variable density,

density=2700,

the material number 1 will still have the old density of 7800. So you must repeat the command:

mp,dens,1,density

Regards,
Alex