Analysis fails: file read/write error?

[Petr.Krysl]

 Running the analysis on a linear statics model I got the following error message (see at the bottom: forrtl: severe (64): input conversion error, unit 23).  Has anyone seen this before?

Thanks,

Petr

Autodesk (R) Simulation Static Stress with Linear Material Models
Version 2013.00.00.0411-W64/X64 28-Feb-2012
Copyright (c) 2012, Autodesk, Inc. All rights reserved.

DATE: JULY 8, 2012
TIME: 06:18 PM
INPUT MODEL: C:\Users\pkrysl\Documents\Autodesk simulations\slot.ds_data\1\ds

PROGRAM VERSION: 201300000411
alg-win-x64.dll VERSION: 201300000411
agsdb_ar-win-x64.dll VERSION: 201300000411
algconfig-win-x64.dll VERSION: 201300000411
algsolve.exe VERSION: 0
amgsolve.exe VERSION: 360000000

**** Linear stress analysis
**** Nodes | Parts | Loads | Freqs | Mode
1968| 1| 1| 0| 0

**** Model Unit System Settings:
--------------------------------------------
Unit System : English (in)
Force : lbf
Length : in
Time : s
Temperature (Absolute) : deg F (R)
Thermal Energy : in*lbf
Voltage : V
Current : A
Electrical Resistance : ohm
Mass : lbf*s^2/in
--------------------------------------------

Options executed are:

NOMIN
STRAIN
SPARSE
SUPCNF
SUPELM
SUPNOD
REAC


processing ...

**** OPENING TEMPORARY FILES
NDYN = 0
**** BEGIN NODAL DATA INPUT
1968 NODES
5904 DOFS
**** END NODAL DATA INPUT

forrtl: severe (64): input conversion error, unit 23, file C:\Users\pkrysl\Documents\Autodesk simulations\slot.ds_data\1\ds.cst
Image PC Routine Line Source
srunx.exe 000000013F9A06E8 Unknown Unknown Unknown
srunx.exe 000000013F99C1B9 Unknown Unknown Unknown
srunx.exe 000000013F9538CF Unknown Unknown Unknown
srunx.exe 000000013F93ADB8 Unknown Unknown Unknown
srunx.exe 000000013F93A4C0 Unknown Unknown Unknown
srunx.exe 000000013F91C19A Unknown Unknown Unknown
srunx.exe 000000013F1D97E2 MPCONSTR_mp_READ1 244 mpc.for
srunx.exe 000000013F1D8E02 MPCONSTR_mp_MPCRE 374 mpc.for
srunx.exe 000000013F2DFAA5 READ_NODES 454 input.for
srunx.exe 000000013F30A0DC PHASE1S 158 wmain0s.for
srunx.exe 000000013F26CD0B MAIN__ 347 srunx.for
srunx.exe 000000013FB0E27C Unknown Unknown Unknown
srunx.exe 000000013F985FDF Unknown Unknown Unknown
kernel32.dll 0000000076DE652D Unknown Unknown Unknown
ntdll.dll 00000000774DC521 Unknown Unknown Unknown

[John_Holtz]

Hi Petr,

I have not encountered that, and I could not reproduce it (based on what I thought it might be related to). The file "ds.cst" is related to multi-point constraints (MPCs). Did you apply these to the model? If so, check to make sure they are correct.

MPCs are also used for cyclic symmetry. Do you have this in your model? If so, check to make sure it is set up correctly.

MPCs are also used for smart bonding ("Setup > Model Setup > Parameters), but since you only have 1 part, there is no need to any type of contact to be specified.

If none of those are the solution, then you will need to archive your model per the thread "Create, Post, or Provide an Archive of your model" and attach it to the Group.

[Petr.Krysl]

Thanks for your reply John.  The archive is attached.

The model does not include multi point constraints, as far as I know.I certainly did not apply them.

Petr

[Petr.Krysl]

Actually, now that I look at the documentation I seem to read the description of the boundary conditions differently: it appears to me now as if frictionless constraint was internally handled as multi point constraint.  Is that correct?

[madg1]

do you have the model fixed? 

[John_Holtz]

Hi Petr,

You (and the documentation 😉 are correct: frictionless constraints are handled using multi-point constraints.

First, have you tried to run the analysis a second time? Some times things happen -- just because they happen.

If it still has the problem, the solution in your case is easy. You can replace all of the frictionless constraints with symmetry boundary conditions. You can do this because all of your sufaces are planar and perpendicular to a global axis. So select the top and bottom faces, "Setup > Constraints > General Constraints > Z Symmetry". Do the same for the left and right faces and assign X symmetry. The front faces gets Y symmetry. (Basically, the axis that is normal to the plane is the type of symmetry constraint to apply.) That should do it.

[madg1]

john

the model is not fixed right?

[John_Holtz]

Hi everyone,

The original model was properly restrained. The frictionless constraints let the surface move "in the plane" of the elements, but they do not permit the nodes to move perpendicular to the plane of the elements. So with three mutually perpendicular side restrained, the model cannot experience rigid body motion. See the attached image.

P.S. I no longer have 2013 installed, and the newer version that I tried did not have a problem with the frictionless constraints. It could be computer related, but I suspect it is fixed in the new, not-quite-yet-released version.

[Petr.Krysl]

John,

Thanks for your response.  I have successfully solved the problem with general constraints replacing the frictionless constraints.  This was the only model out of a line of several examples which had a problem with the frictionless constraint, although none have as many as this one (with Simulation Mechanical 2013).

The documentation does not actually spell out that the friction was constraints are enforced as multi point constraints in any other place but in the discussion of multi point constraints.  When I get a chance I will try to add that information on the wiki page.

Petr

[madg1]

P.S. I no longer have 2013 installed, 

you mean 2012 right.

that makes sense...i m opening model in 2012.....so thats bad...