Query on Abaqus *fil file

[Tinni1]

Hi,

I have a query regarding importing imperfection from linear buckling analysis.

I have provided command in the edit keyword section as below:

Node File,
U
As I understand that if I conduct a linear buckling analysis, then a *fil file will be generated which contains the coordinates of the normalized eigen modes obtained from the linear buckling analysis.

In my case, a FIL file is generated in a text pad format. But when I am opening the file it is not showing any coordinate instead shows some unknown characters that I am unable to understand.

I am attaching the FIL file here.

Could anyone provide any direction, why I am not able to see the coordinates in the *fil file?

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1641498689/tips/Job-1_rfieil.fil[/url]?

 

[FEA way]

That's a legacy format with binary output, it's meant primarily for use in external postprocessors. If you want to read the values, you should use another output format - dat file:

*Node Print
U

 

[Mustaine3]

It is possible to switch the file format from binary to ASCII with this command:
*File Format, ASCII

 

[Tinni1]

Thanks for your response.

@ Mustaine3
Could you please let me know, where should I write the command in the edit keyword section?
Is that like below?
*Node File,
U
*File Format, ASCII

Thanks in advance.

 

[FEA way]

Yes, you can do it this way. Just remove the unnecessary comma:

*Node File
U
*File Format, ASCII

 

[Mustaine3]

It's ok that way.

Quote from the documentation:
"The *FILE FORMAT option can be given as model data or as history data, but it can appear only once in the input file."

 

[Tinni1]

Great! many thanks!

 

[flyforever85]

What would be the procedure for EXPLICIT? I keep reading the manual with no success. The only info I've been able to find is to write convert=select but I lunch my analysis in a cluster and I don't have that option.

 

[FEA way]

In Abaqus/Explicit you have to use the .sel (selected results) file instead of .fil or .dat files. After the analysis, the .sel file can be converted to .fil using this command:

abaqus convert=select

 

[flyforever85]

that is from command line only, correct? Any option available to transform the sel into fil within the *.inp file?

 

[FEA way]

Yes, it’s like the command that you use to submit the job (e.g. abaqus job=…). It can’t be done from the input file but it shouldn’t be a problem to submit such a command even when running the job remotely.

 

[flyforever85]

I found how I can add that to the cluster bu that's what I receive:

job=XYZ.inp convert=select cpus=32 memory=30720MB interactive
b'Abaqus Error: Command line option "scratch" may not be used with "convert".'

According with the manual the two commnad (scratch and convert) are not mutually exclusive. Also I'm not using scratch so I really don't know what should I change

 

[FEA way]

Try without the additional parameters, just this:

abaqus job=job_name convert=select

 

[flyforever85]

Unfortunately I cant, I use a cluster so some paramters are there by default, I can only select how many cpus to use, but cant' get rid of the cpu command. It's nervewrecking because I have a .sel file I just can't read it

 

[FEA way]

What about the other parameters - can't you remove them ? Another option would be to copy the file and convert it locally if you have a license for that.

 

[flyforever85]

I'm trying to convert the sel into ASCII on my computer. Difficult as well since I can't install any .exe