Error ID 54 - Radioss
I'm trying to run an analysis in Radioss and I get an 'Error ID 54'. Together with some more errors and warning. I attach the .out file (complete)
ERROR ID : 54
** ERROR IN INPUT FORMAT
DESCRIPTION :
IN BLOCK : 581 588 589 590 591 592 593 594 595 596
Thanks for helping
Answers
-
Hi,
Use Tools>Model Checker>RadiossBlock to find modeling errors.
https://insider.altairhyperworks.com/wp-content/uploads/2017/09/T-T-1248-HyperMesh-Model-Checker.pdf
Share the model if the issue persists.0 -
I did that. Now I don't get errors in model Checker (I do get warning such as 'free nodes in the model', 'incompatible kinematic conditions on nodes', 'Rbody id is different from master id' and 'Rigid body connected to only one part').
But I still get the same error
ERROR ID : 54
** ERROR IN INPUT FORMAT
DESCRIPTION :
IN BLOCK : 581 588 589 590 591 592 593 594 595 596I send the file attached
Thanks
0 -
The following modifications were made:
-for plane strain analysis, the elements must be defined in YZ plane and their normals have to be in the positive x-position, so the model was reoriented
-P1_SHELL property is not allowed so it was changed to P14_SOLID
-SHELL element type is not allowed so was changed to QUAD using 2D>elem types>2D & 3D>quad4 + pick all elements and update
Rigid bodies were placed in a separate component without Part card image. However, rigids are not allowed in this type of analysis, so they should be deleted.
ERROR ID : 638
** ERROR IN INPUT CONSISTENCY
DESCRIPTION :
RIGID BODIES ARE NOT COMPATIBLE WITH 2D ANALYSIS1rigid bodies also cause error 54
0 -
Thanks!
I'll check it and write you back
0 -
Thank u so much. How do u think I could delete the rigid body but remain what I need?:
- The center of that rigid body to be the center of rotation
- The inner nodes of 'pinon' and 'rueda' to be fixed on the 6dof with respect to that center of rotation
Thanks again!
0 -
Actually, RBE2 elements can be used.
Contact interface type 3 is set up with contact surfaces.
Simulation controls are defined by utility>engine file assistant.
The moment load is linearly ramped up to avoid inertial effects.
A coarse (automesh) and fine model is attached.
Note after 8e-3 seconds for some reason there are severe deformations.
0 -
- Is it necessary to change all the loads as u did? The 'rueda' was supposed to be rotating some degrees during each step (quasi-estatic analysis), while the pinon had a moment.
- Why are all the noded from rueda and pinon blocked in all DOF but the rotation in Z?
- Can't the moment be applied as it was before (you created a curve to do it)
Thanks a lot and sorry for so many problems,
0 -
You're welcome. The Like button is an easy way to show appreciation
/emoticons/default_wink.png' srcset='/emoticons/wink@2x.png 2x' style='border-style:none;vertical-align:middle;' title=';)' width='20' />
1. I have overlooked that rueda had prescribed motion. Use Utiliy>BCs manager>Imposed displacement or Imposed velocity to set up a rotation on the master node of RBE2 element of rueda. (XX axis of rotation).
2. Rueda and pinion have blocked all DOF except X axis rotations (similar to the original model). This allows the moment to act on pinion, avoids incompatible condition on rueda and prevents rigid body modes.
3. If the moment load is applied suddenly (without ramp up) it will induce inertial dynamic effects becoming impact analysis instead of quasistatic.
Following the unit consistency of N, mm, ton, s the moment load is 200.000 Nmm- is this correct?
0 -
Yep 200.000 N·mm (200 N·m)
0 -
To obtain a steady state, quasi-static analysis both gears should be fully modeled to stay in contact throughout rotation, imposing constant velocity on rueda and gradually ramping up the moment load on pinion.
Also check the following example:
https://altairuniversity.com/wp-content/uploads/2012/08/Example_15.pdf
0 -
I have no idea of how to create a constant velocity on the rueda and a ramping up moment on the pinion
0 -
I guess I have to créate a curve first but I get this error when I click 'new' on 'curve editor'
while executing
'hm_getstring 'Name =' 'Create a new curve''
(procedure '::HMCurveEditor::onNewCurve' line 6)
invoked from within
'::HMCurveEditor::onNewCurve'
('eval' body line 1)
invoked from within
'# Compiled -- no source code available
error 'called a copy of a compiled script''
(procedure '::hwt::ReleaseCanvasButton' line 1)
invoked from within
'::hwt::ReleaseCanvasButton 0 .ceWindow.actionFrame.newButton'
(command bound to event)
0 -
Problem solved. Anyway, I still don't manage to get what I needed
0 -
Everything needed to set up boundary conditions with curves is explained in the video already shared (7 Guidelines to apply Quasi-static Load in Explicit Simulation). The only difference is constant velocity is applied with Imposed Velocity and ramping up moment load with Concentrated Load. I could do it for you, but you will only learn by doing it yourself.
Creating curves is also covered in that video. Alternatively, curves can be set up with XYPlots>Curve editor. I have not yet faced the error you mentioned. Can you share some screenshot and software version you are using?
Can you be more specific what is the problem exactly you need to get resolved? If possible share the working Optistruct model (the one you shared has many issues and could not be run), or at least explain the problem.
0