Robot Structural Analysis Forum
Welcome to Autodesk’s Robot Structural Analysis Forums. Share your knowledge, ask questions, and explore popular Robot Structural Analysis topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Time History Analysis

18 REPLIES 18
Reply
Message 1 of 19
ianrhale
2217 Views, 18 Replies

Time History Analysis

I have three questions about this file, i will start with the easiest as the last may be difficult to answer. Number 3 is the main issue.

 

1) I have applied a load to N3 as 1-Wind and a load to N3 as 2-Wind TH. When viewing the load diagrams the first is on its own as it should be, but in 2-WindTH it seems to combine the two loads, as if i have made them a combination. I can't see why this is happening.

 

2) I'd like to remove the roller at N4 as it does not allow accurate modelling of the system, but as two cables are joined here i can't see how. Perhaps a rigid link, or coupled nodes?

 

3) There is a time history loaded into the file. This represents wind speed, but by applying a small load factor, say 0.03, I can 'convert' this to a load in kN. So essentialy, the time history is a force. I wish to apply this in the X direction to N3. I have tried to apply the principle I have seen on the falling object example which I have seen Pawel linked in a previous post, but have got myself confused. My main questions are how do i 'tell' Robot this is a force in X (as opposed to an accelleration or displacement), and how do i tell Robot to apply it to N3?

 

I have tried to acheive this as can be seen in the file, but i'm really not sure if this has worked out at all. (The small load factor is not yet included).

 

Many thanks in advance!

18 REPLIES 18
Message 2 of 19
Pawel.Pulak
in reply to: ianrhale


@ianrhale wrote:

1) I have applied a load to N3 as 1-Wind and a load to N3 as 2-Wind TH. When viewing the load diagrams the first is on its own as it should be, but in 2-WindTH it seems to combine the two loads, as if i have made them a combination. I can't see why this is happening.

 


In case of structures containing cables the 1st load case is treated in Robot as the assembling load case and it is automatically added to all other load cases.
It is discussed in this forum topic:
http://forums.autodesk.com/t5/Robot-Structural-Analysis/structure-par-phase-cables-assembling-load-c...

The effects of it can be seen in both data and results of your model:

cable2.png

 


@ianrhale wrote:

2) I'd like to remove the roller at N4 as it does not allow accurate modelling of the system, but as two cables are joined here i can't see how. Perhaps a rigid link, or coupled nodes?

 


After removing the roller in node 4 cables 4 and 5 will create a collinear chain so it is recommended to activate geometrical 3rd order effects for load cases ("P-delta analysis" check-box responsible for it).  It may ba also necessary to activate matrix update after each iteration in paramaters of nonlinear THA.

It is not necessary to define rigid links or coupled nodes.


@ianrhale wrote:

3) There is a time history loaded into the file. This represents wind speed, but by applying a small load factor, say 0.03, I can 'convert' this to a load in kN. So essentialy, the time history is a force. I wish to apply this in the X direction to N3. I have tried to apply the principle I have seen on the falling object example which I have seen Pawel linked in a previous post, but have got myself confused. My main questions are how do i 'tell' Robot this is a force in X (as opposed to an accelleration or displacement), and how do i tell Robot to apply it to N3?

 

I have tried to acheive this as can be seen in the file, but i'm really not sure if this has worked out at all. (The small load factor is not yet included).

 


Generally time functions in time history in Robot are unitless - except of virtual load cases "DirectionX", "DirectionY", "DirectionZ" described in the message 2 of this forum post: http://forums.autodesk.com/t5/Robot-Structural-Analysis/great-work/td-p/3729078
So if time functions are unitless it means that excitements have the units of loads defined in load cases used in THA.
In your model the unitless time function WIND_TH is used for load case 2 which contains the horizontal force FX=1 kN applied to node 3.
It means that the excitement is a horizontal force changing in time t according to function 1 kN * WIND_TH(t).

In my answer to point 1) I have mentioned that the assembling load case as is automatically added to all other load cases. In concerns also the time history load case, but here this component is not multiplied by time function - it is treated as the constant component of load.
In your model the assembling load case contains selfweight and some wind load modeled as the horizontal force FX=0.5 kN applied to node 3

The simplest approach seems defining the average value of wind load in the assembling load case while the value in load case 2 and WIND_TH will be responsible only for time-dependent oscillations (positive and negative) from the average value.

 

---------------------------------------------
If this post answers your question please click the "Accept as Solution" button. It will help everyone to find answer more quickly!

 

Best regards,



 


Pawel Pulak
Technical Account Specialist
Message 3 of 19
ianrhale
in reply to: Pawel.Pulak

Pawel,

 

Thanks for your reply - it cleared up how to apply the time history. It has raised a few more questions however.

 

1) The model is now very slow to interrogate, switching between results cases, creating diagrams etc, I wonder if i have created too many data points somewhere in my TH analysis? Analysis takes about 1 minute, which is as expected.

 

2) In the post linked below I had an issue with materials (I will pay the fine!). In this model I have defined the materials under the steel tab but they still do not appear in the cable definition dialog.

 

http://forums.autodesk.com/t5/Robot-Structural-Analysis/Tension-Model-Problem/td-p/4758375

 

3) If a static horizontal load is applied, the two colinear cables do not seem to form a straight line under the deflected shape which seems strange.

 

4) In my TH diagrams, there is a diagram plotting the force in the two cables over time. The diagram seems to be telling me I have very disparate forces in the two cables? I am expecting differing values as one is intended to be an elastic 'shock' link, but not to this magnitude. Also, the reaction TH diagram gives me no values as far as I can see so it is hard to check this. My TH has values of about 10, my force applied to the node 0.17kN so I am expecting forces of magnitude around 1-5kN perhaps.

 

Thanks, Ian.

Message 4 of 19
Pawel.Pulak
in reply to: ianrhale

ad 1) and 3)

When trying to open your model Robot has hung - it was necessary to kill it.

I have managed to open it in reapir mode but there was no load case 1. Have you deleted it by mistake?

In such situation case 2 is treated as the assembling one. No loads on cables (like selfweight for instance) in this load case result in considering cables during analysis as standard truss members.

You have also not activated P-delta for time history.

When I have run analysis instability and matrix non positive definite was reported and then the nonlinear time history was not convergent. When trying to display results Robot has hung again.

 

Breaking analysis during THA I was able to see results for case 2 - abnormal shape of deformation is justified by abnormal values of it (close to 1500mm) and by considering cables as truss members

 

ad 2)

As I see you have overwritten material definition from the definition of cable (CABLE HOVET) by material directly assigned to element in the table of bars (materials displayed in this table in italics Elastic and Polyester mean materials assigned directly to elements and owerwriting the original ones).

materials.png

It is recommended to avoid such overwriting - if Elastic and Polyester material are defined in material database on your computer you should be able to assign them directly in New Cable window.

Just after defining new materials it could be so that you were not able to see and select them - in such case it is necessary to save the model and restart Robot  to be able to  see and select them.

 

ad 4)

THA was not convergent so difficult to discuss results.

 

Attached your model with case 1 restored, activated P-delta and stiffness update after each iteration for time history.

This time analysis run wiithout any error messages.

 

Regards,

 

 

 


Pawel Pulak
Technical Account Specialist
Message 5 of 19
ianrhale
in reply to: ianrhale

Pawel,

 

Thank you for the file. I am not with the computer that has Robot at the moment, i will take a look tomorrow.

 

There was no indication during the analysis that the TH did not converge - the analysis appeared to run ok. Also, when i restarted Robot the materials did not appear in the list - and I have never seen 'CABLE HOVET' material before until just now!

 

As a beginner with Robot, I can misunderstand certain things so thanks for your patience.

Message 6 of 19
ianrhale
in reply to: ianrhale

Pawel,

 

I have had a look over the file, and modified it slightly to simplify it by using only one material for the cables. No matter what I do, I cannot get the materials 'elastic' and 'polyester' to show up in the cable dialog box, so I have to set them to S235 and over-ride them.

 

Now I have some results, I can see by working through the time steps that the method applies a force to the node which is of the magnitude I require - in the region of 1 to 2kN. Obviously the model is showing large deflections which feels wrong to me, particulary as at some points in the TH the force in the members is hundred or throusands of kN. Is this due to my method of applying the load? I find it hard to grasp how a force of around 1 kN, varied over time can create such forces in the structure?

Message 7 of 19
Andyf88
in reply to: ianrhale

Hello, 

 

I have kind of the same exercise but my problem is that even though I am applying a TH load lasting only 0.11 s, see the time function definition in th pic, the structure continues the oscillations even after 1 s. I have applied the dumping factors similar to the example that you have given. But still even without damping, shouldn't it almost stop after 0.11 s?

 

If anyone can help I would be very grateful.

 

 

 

 

Time Function

Message 8 of 19
Pawel.Pulak
in reply to: Andyf88

Depending on the value of damping the speed of dissipation may be different.

It is not abnormal that the visible oscillations are observed after the time 10x longer that the time of the excitation.

 

Without damping theoretically it is possible that vibrations will never dissipate.

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 9 of 19
Andyf88
in reply to: Pawel.Pulak

Hello Pawel,

 

Thank you for your reply.

 

It makes sense what you are saying. It's just that I did the exercise using hand calculations and I go the oscillations reducing significantly after the load stops (after 0.11 s). And I was expecting a result like this example:

 

Untitled 1.png

 

 

 

Which I found in this forum:

 

http://forums.autodesk.com/t5/robot-structural-analysis/problems-with-time-history-analysis/m-p/3488...

 

 

I guess, someone might argue that it depends on the damping coeficients that have been used in this example.

 

Any comment is appreciated.

 

 

Message 10 of 19
Pawel.Pulak
in reply to: Andyf88


@Andyf88 wrote:

I guess, someone might argue that it depends on the damping coeficients that have been used in this example.

 

Any comment is appreciated. 


It depends not only on the damping but also on the type of excitement and properties of the structure.

It the example given by Rafal the excitement is harmonic and the vibrations during the excitement are practically steady-state forced harmonic vibrations with some frequency.

When the excitement stops the structure automatically "returns" to free vibrations with own vibration frequencies which can be (and the screen capture from Rafal's post shows that they are) significantly different than the frequency of excitement. Moreover the shape of own free vibration modes can be completely different than the shape of forced vibrations. It usually results in fast change of response just after stopping excitement - as on the screen capture  from Rafal's post . After this sudden change there is a zone of slower reduction resulting from damping.

 

In your case the excitement was not harmonic or periodic but rather impulsive/short-time and moreover it was decreasing in time. The shape of the diagram suggests that it rather only initiated free vibrations - with relatively slow reduction/dissipation resulting from damping.

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 11 of 19
Andyf88
in reply to: Pawel.Pulak

That is true and comprehensive Pawel, thank you very much, you were very helful.

Kind Regards
Message 12 of 19
Andyf88
in reply to: Pawel.Pulak

Pawel,

 

Sorry, I just have another question.

 

In the first case I showed to you I had used a Newmark method for the Time History Analysis.

 

In the case showed in th epicture below I am using Modal Decomposition method, but the results are so different from each other.

 

Why does this happen, and which ishould be most reliable one?

 

 

Untitled123.png

Message 13 of 19
Pawel.Pulak
in reply to: Andyf88

Modal decomposition is defined without any damping - to compare it with Newmark method it would be necessary to define similar damping.

Moreover the number of modes in modal analysis is important in modal decomposition method - especially in fast changing response

And your screen captures suggest that in modal decomposition the forcing functions were related to cases 4 5 and 6 while in Newmark method only the case 4.

and... (difficult to say/guess without your models)

 

Regards,

 


Pawel Pulak
Technical Account Specialist
Message 14 of 19
Andyf88
in reply to: Pawel.Pulak

Pawel,

 

Even when I use the 3 cases it is something similar, see the picture below.

 

I am sending you also the robot file to check if possible. You can find it in here:

 

https://dl.dropboxusercontent.com/u/44309793/PCR%203D%20%20-%20Comb%20TH%20Loads%20(D-drive).rtd

 

Many thanks.

 

 

Untitledsdsd.png

Message 15 of 19
Pawel.Pulak
in reply to: Andyf88

It was my most suitable guess for your model: "Moreover the number of modes in modal analysis is important in modal decomposition method"

 

You have probably run THA decomposition method for the setting of modal analysis used  in the model uploaded via dropbox - the default number of 10 modes.

 

But when checking results it can be seen that all vibration frequencies are very close and moreover the participation mass percentage is very low - see below. It suggests that these modes correspond to mostly some local vibrations, not related to global vibration of whole structure.

mass1.png 

 

The precision of results for modal decomposition method depends on the number of modes considered (and whether their shapes correspond to the response of the structure to given excitement). As the name suggests the response is "built"  or composed from modal responses.

 

Your original model contained only THA case using the Newmark method - case 7. To easily observe the difference between the Newmark method and the modal decomposition method I have added in this model another THA case using the modal decomposition method - case 11. I have used in it the parameters analogous to case 7 - no damping, the same forcing functions, starting case, integration time, etc....

When such model was run with 10 modes the comparison of analogous results has shown very significant differences - as below:

10modes.png 

 

But after increasing the number of modes in modal analysis to 50 it looks much better:

50modes.png 

 

And when using 100 modes it is difficult to see any difference between cases 7 and 11:

100modes.png 

 

So it could be told that the Newmark method is better because it does not need to take care about the number of modes to obtain correct results But it is not so simple (as usually in dynamics:)) because:

  1. even with 100 modes modal decomposition is much faster than Newmark method for your model
  2. while modal decomposition is sensitive to the number of modes considered the Newmark method is sensitive to the size of integration steps (Time step/Division). Not observed in this model but generally such property exists

I have also attached the model modified as above - without results to reduce its size.

 

I have additional remark related to your model - modal analysis is defined to consider only the mass of the structure . There is no load to mass conversion and the load case 1 contains also some other loads than self-weight (and moreover self-weight is considered for some elements twice). If these additional dead loads should be considerd in dynamic analysis as masses it is necessary to define load to mass conversion and activate "Disregard density" in modal analysis.

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 16 of 19
Andyf88
in reply to: Pawel.Pulak

Pawel,

You are great, THANK YOU!

The duplicated loads were a mistake, which I corrected.

In case 1 i have added "self weight" and "dead load from roof".

1. Do you think I should add case 1 in the load mass conversion? What about live load? And what parameters would be best? e.g. "Conversion direction" = Z-; "Add mass to" = "Dynamic mass".

2. And if I activate "Disregard density", then the density of the material will be 0 and won't calculate the self weight of the members, isn't it true?

3. Also, do you think this is the best way to combine 3 TH loads as I have done.? My intention was to create a realistic blast load, with the pressures applying on 1. front wall, 2. roof, 3. side wall simultaneously but with different functions. So I had to combine the 3 of them plus the dead load. The only way I found was to add the 3 of them in one THA analysis type and put case 1 as for the option "Consider results for a selected case as initial ones". Is there any other/better way to do this combination? Can I combine them as I do with the static loads where I can put factors as well?

I hope I was clear, and thank you for your time.
Message 17 of 19
Pawel.Pulak
in reply to: Andyf88


@Andyf88 wrote:

In case 1 i have added "self weight" and "dead load from roof".

1. Do you think I should add case 1 in the load mass conversion? What about live load? And what parameters would be best? e.g. "Conversion direction" = Z-; "Add mass to" = "Dynamic mass".

2. And if I activate "Disregard density", then the density of the material will be 0 and won't calculate the self weight of the members, isn't it true?

 

Here is how it is set in the files received from you and sent back to you by me:

no_load_to_mass_conversion.png

 

Such settings results in considering in dynamic analysis only the mass of the structure.

 

If not only the mass of the structure should be considered but also the mass related to other dead loads from load case 1 then the setting shown below should be used:

load_to_mass_conversion.png

 

In this setting "Disregard density" (in other words "Disregard mass of the structure") is activated but it is "replaced" by converting to mass the self-weight load contained in load case 1. Additionally the uniform load of 1.35 kN/m2, applied to claddings, is also converted to masses.

 

If live loads also correspond to masses and they will exist during the blast then no problem to consider them too - adding them to load to mass conversion completely (coefficient 1.0) or partially (coefficient < 1.0)

 


@Andyf88 wrote:
3. Also, do you think this is the best way to combine 3 TH loads as I have done.? My intention was to create a realistic blast load, with the pressures applying on 1. front wall, 2. roof, 3. side wall simultaneously but with different functions. So I had to combine the 3 of them plus the dead load. The only way I found was to add the 3 of them in one THA analysis type and put case 1 as for the option "Consider results for a selected case as initial ones". Is there any other/better way to do this combination? Can I combine them as I do with the static loads where I can put factors as well?

The way to model the blast is a good one. It is possible to model it considering additionally the speed of the pressure wave but it seems not necessary in this case.

Static loads can be considered activating "Consider results for a selected case as initial ones" as you did.

It is also possible to convert specific time steps ot time history to simple cases and then to combine them with other cases. It is discussed and shown at the end of this post:

http://forums.autodesk.com/t5/robot-structural-analysis/definition-of-blast-accidental-loads-in-robo...

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 18 of 19
Andyf88
in reply to: Pawel.Pulak

Very precise and helpful everything.

Many thanks Pawel, wish you all the best.

Regards.
Message 19 of 19
9tuplesys
in reply to: Pawel.Pulak

Hi guys!

 

I downloaded the example of the steel structure from above and I modified the analysis as follow:

- case 7 - TH over Direction X/Y/Z

- case 11 - TH over static cases 4, 5 and 6

Please have a look on Loads to mass conversion, too.

 

My question is why the response of the structure starts in a different way: for case 7 from zero and from case 11 from a certain value. I expected to have more or less same results from both situations.

Here is the link to my analysis file:

https://www.dropbox.com/s/yepywt2j967jhgi/PCR%203D%20%20-%20Comb%20TH%20Loads%20%28D-drive%29pp3_wit...

 

case 7case 11

 

TH-comp.JPG

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report