Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

NLGEOM - constant and non-constant loads

Andrea_22029

Hi everyone,

I am trying to run a Geometric Non-Linear (implicit, NLGEOM) in Optistruct, and I found a difficult in applying loads.

I can run a simulation of a table-defined load without any problem (defining force->table->nload1->nload); but I do not know how to apply a constant load to the varying one.

For example: I've to apply both gravity and pressure loads on an inflatable beam, and after that I would apply a pattern of force definet by a table. I tried to define a table like that for pressure:

0.0 1.0

1.0 1.0

2.0 1.0

but I find an error of no-convergence, probably due to the initial step. I could not find any tutorial about that.

Now I want to ask you: can I define a constant pressure load to perform the NLGEOM analysis? Or I have to define the pressure-table like that:

0.0 0.0

1.0 1.0

2.0 1.0

and after time 2.0 apply the variable load?

Thank you for your attention.

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

Adriano_Koga

Hi @Andrea

Is there any particular reason for using this Implicit NLGEOM option?

I ask you this because it is kind of 'discontinued' option, as in the past it used to convert the model and run internally using Radioss.

Now that OptiStruct has all the NL stuff, you can just run a NLSTAT analysis type. In NLSTAT you can define a varying load by sing a similar setup (TABLED1,TLOAD1,DLOAD)

Or you could create 2 sequential steps:

1) NLSTAT, with Gravity+Pressure (Combined through LOADADD)

2) NLSTAT using CNTNLSUB (continuation from loadstep1), keeping the Gravity+Pressure (LOADADD), and adding the varying load with the TLOAD1/DLOAD

I believe something like this would be what you're looking for.

For convergence issues, NLADAPT can be used for better handling increments, and other controls.

Andrea_22029

Hi @Andrea

Is there any particular reason for using this Implicit NLGEOM option?

I ask you this because it is kind of 'discontinued' option, as in the past it used to convert the model and run internally using Radioss.

Now that OptiStruct has all the NL stuff, you can just run a NLSTAT analysis type. In NLSTAT you can define a varying load by sing a similar setup (TABLED1,TLOAD1,DLOAD)

Or you could create 2 sequential steps:

1) NLSTAT, with Gravity+Pressure (Combined through LOADADD)

2) NLSTAT using CNTNLSUB (continuation from loadstep1), keeping the Gravity+Pressure (LOADADD), and adding the varying load with the TLOAD1/DLOAD

I believe something like this would be what you're looking for.

For convergence issues, NLADAPT can be used for better handling increments, and other controls.

Hi @Adriano A. Koga

thank you very much for your answer.

I was using implicit non-linear because it is the only option I knew that allows to apply a variable load without considering inertia-terms.

The main purpose is to set-up a model and use it in HyperStudy in order to fit the force-displacement response of the model on experimental data varying the Young Module E of the material. I would try to do something like the HS-1506 tutorial in HyperStudy, and for that I need that the model outputs a curve of displacement through some forces I have chosen.

I would use NLSTAT, but I didn't know how to get a curve-responce unless defining a lot of loadsteps, which is very time-expensive.

Perphaps my way is not the best one, but now I will try to define a TALBLED1 load in a NLSTAT analysis.

Thank you again.

Adriano_Koga

Hi @Adriano A. Koga

thank you very much for your answer.

I was using implicit non-linear because it is the only option I knew that allows to apply a variable load without considering inertia-terms.

The main purpose is to set-up a model and use it in HyperStudy in order to fit the force-displacement response of the model on experimental data varying the Young Module E of the material. I would try to do something like the HS-1506 tutorial in HyperStudy, and for that I need that the model outputs a curve of displacement through some forces I have chosen.

I would use NLSTAT, but I didn't know how to get a curve-responce unless defining a lot of loadsteps, which is very time-expensive.

Perphaps my way is not the best one, but now I will try to define a TALBLED1 load in a NLSTAT analysis.

Thank you again.

in fact you could combine all of them into a single DLOAD (Gravity + Pressure + loading), and haivng a single loadstep, as well.

You need to have 3 TABLED1's, 3 TLOADs and 1 DLOAD combining them all.

your GRAV and PRess will start at the very beginning (with a linear slope), and then later on, the varying load can be turned-on.

Adriano_Koga

in fact you could combine all of them into a single DLOAD (Gravity + Pressure + loading), and haivng a single loadstep, as well.

You need to have 3 TABLED1's, 3 TLOADs and 1 DLOAD combining them all.

your GRAV and PRess will start at the very beginning (with a linear slope), and then later on, the varying load can be turned-on.

just in case you need, a sample model, with TLOAD nad TABLED1 for NLSTAT.

For multiple TLOADs, combine them through DLOAD

chair_nofllwer_timedependent.fem