HelpDesk
sign in

MOVING LOAD CASE DEFINITION

Creation date: 10/3/2018 11:00 PM    Updated: 10/4/2018 8:52 AM
Print...
Question:

             Hello dear friends,

I have modeled a bridge with 3 spans and I want to design the elements about Eurocode. The combinations
were automatic generated about the program but it is something strange because when I select just the moving
load defined (MV , you can see in the attached screenshot) the program don't gives me the diagrams My in the
precast beams (post-tensioned beams). In the same time I want to ask you how can I determine the moments on the
top and bottom of the plinths for rebar designing.

Best regards and thank you very much.


Answer:

        
                   Hello dear Gohil,

in the model I sent you, please help me to define the stage constructions. I have define next groups:
Stage 1- piles an plinth  - foundations group; - duration 60 days;
Stage 2- pier elevation and pier cap - elevations group;- duration 60 days;
Stage 3-  mounting precast beams - beams group - duration 10 days;
Stage 4- cast in situ concrete in cross beams: - duration 28 days - cross beams group;
Stage 5- cast in situ concrete in the overlay(firstly wet concrete): - duration 30 days - dummy group;
Stage 6 - composed section(precast girder + overlay) , to which is applies the road structure self weight and traffic load
Thank you very much.

Best regards


Hello,

So, first lets see the issue with moving load.  Actually the structure group selected for cross beams was not proper.  The CROOBEAMS should have all the elements as highlighted in the image below (Deck & diaphragm) .  With that, the results would be as expected.  Moreover, the closer the spacing of cross beams, the better.  I believe a spacing of about 1m to 1.5m would give better results of bending diagram.


For construction stage, the structure groups are defined property, but the boundary groups are not proper.  For instance, only one group LINKS is created.  But the connection between pier and pier cap will not be activated in the same stage as connection between girder and pier cap.  So, multiple boundary groups need to be created accordingly.
A modified sample model is attached for review in which stages are defined.  Though, composite section fro construction stage is only defined for one section.  That has to be done for all longitudinal sections.
Kindly let us know if further assistance would be required.

Regards,
Nandeep
Technical Manager, MIDAS


        Hello dear Nandeep,
 
  thank you very much for the last response you sent me, I understood you indications, but for example if I want to
  have directly the bending moments(without stage construction) it is possible? In the model I have attached in this
 email I have obtain correctly the diagrams My in beams(moving load combination, I have modified in lane definitions the
 elements for transversal distribution  including cross beams and dummy elements, please see the diagrams in the first
screenshot) but I think that I not obtain correctly the diagram for Eurocode load combination concrete design (cLCB1, please see
the second screen shot attached). I think that the dummy elements are not active for transversal load distribution in the Eurocode load 
combination. Probably tomorrow I will send to you a question about stage construction, now I am working on this.
Thank you very much.

Best regards,


Hello,

Well, in such a structure, I wouldn't recommend to take forces without construction stages, since there are some loads which start acting in pre-composite state while some start acting after.  Moreover, there are phenomena like differential creep & shrinkage between slab and girder.
The results without construction stage would be very crude approximation.
The cross beams are acting for all the loads.  But since all girders have similar loading, the forces in cross beams would be quite low.  One mistake here however, is the consideration of wet concrete load in the combination.  Since the girder section is composite and we are already considering the density of slab material there, Wet Concrete load case shouldn't be a part of load combination.  The slab weight is considered twice right now.
Besides that, the modelling is fine.

Regards,
Nandeep
Technical Manager, MIDAS


 Hello dear Nandeep,

Thank you very much for all, but I have a new question about stage construction.
I have defined in this phase just first two stage constructions:
- CS1 exactly like your indications (foundations and elevations with own springs groups) ;
- CS2 like in the attached model (the beams are poststressed when we mount them with crane on the infrastructure, that's why I included in CS2 the effect of the poststressed cables and of course the deck links;
The problem is that I perform the analysis. The diagrams in CS2 are not correct (you can see in the second screenshot attached).
Please tell me if I have made something wrong.
Best regards,


Hello,

Glad to be of help.
Actually in the model that's sent, the structure groups are not proper.  Kindly refer the image below.
Add the abutment support locations and nodes at elastic link for bearing to the Foundation structure group.  Besides this, the elastic links should have negligible rotational stiffness for structural stability.  Kindly provide the same as say about 10kNm/rad.
Once this is done, the results are fine.  The modified model is attached for further review.

Regards,
Nandeep
Technical Manager, MIDAS


Hello dear Nandeep,

Thank you very much, I have succeeded and now is ok. Tell me please why exactly the value of 10 kN/rad for rotational values of the Srx, Sry and Srz? It is a particularity of the program?
Another question: why we don't include the bearings points on the elevation group? Is there any reason to include the bearings and abutment supports points only in the foundations group?
Thank you very much my friend.
Beste regards



Good morning dear Nandeep,

I have defined the second construction stage CS2 as you can see in the attached screenshots, but when I perform analysis in this stage CS2, I think that the dead load of the beams is not in action, You can see that on the screenshots attached just the effect of the prestressed cables. My question is that the program recognize automatically the dead load of the beams, because in CS2 the program
does not allow me to assign the dead load in the dialog box of CS2-Load (you can see in the CAPTURE 2 -CS).
I have another problem, after I perform analysis and I want to go back on the pre-processing mode (I press the icon with pre-processing mode). The program does not allow me to make modifications in the construction stage defined, is active just "Show" button.
Thank you very much again and best regards.


Hello dear Nandeep,

For the CS2 (the beams are prestressed when will be put on the infrastructure with crane and naturally just self weight of the beam is active and prestressed force). I have managed to activate the self weight of the beams just if i defined "Beams self weight group" and I have introduced manually the forces of the beams self weight (please see the screenshot attached). In this case I think that the diagrams are correct for CS2 but the deformations of the beams are huge. Please see the model attached and the screenshot. Probably I have made something wrong and I have to correct.
Thank you very much again and best regards,


Hello,

Glad things are proceeding quickly at your end!  I'll try to respond to each issue below:

1)  Tell me please why exactly the value of 10 kN/rad for rotational values of the Srx, Sry and Srz? It is a particularity of the program?
A:  This is just a nominal value.  For stability purpose and to avoid undue warning messages.

2)  Why we do't include the bearings points on the elevation group? Is there any reason to include the bearings and abutment supports points only in the foundations group?
A:  Actually the abutment supports and the pier supports are in the same boundary group.  Now, this boundary group is activated in first stage itself.  Hence, I advised to add abutment supports in first stage.  As for bearing nodes, these could be activated in second stage as well, if required.  But since its just activating the nodes without any connectivity, it wouldn't affect the overall behavior, thus I added it in Foundations group.

3)  My question is that the program recognize automatically the dead load of the beams, because in CS2 the program does not allow me to assign the dead load in the dialog box of CS2-Load(you can see in the CAPTURE 2 -CS).
A:  Actually the DEADLOADS load group is already activated in first stage, thus it can't be added again in second stage.  But in second stage, the beams are activated to which some element beam loads are assigned.  Thus, these loads would have to be added to a load group other than the DEADLOADS.  I created a DEAD2 load group for this purpose.  Temperature loads under Dead Load case have not been added to any load group, hence I made no change there.  Kindly check the attached model.  Also, the beam dead load is already acting.  To check this better, I activated an option to save result of load in each stage.  It could be noted in the image below that in second stage, there is deflection due to just dead load in downward direction.

4)  I have another problem, after I perform analysis and I want to go back on the pre-processing mod(I press the icon with pre-processing mode) the program does not allow me to make modifications in the construction stage defined, is active just "Show" button.
A:  To make changes in construction stage, i.e., see that Modify button, you need to be in the base stage.
As for deformations, I believe these are quite OK based on the assigned forces.  Kindly note that the deformed shape is quite exaggerated.
Kindly let us know if further assistance would be required.

Regards,
Nandeep
Technical Manager, MIDAS

   
Hello dear Nandeep,

I have finished the stage construction and I understood all for this stage. Finally the program generated me a load combination
about Eurocode (I want to design the reinforced concrete about Eurocode) but I have next questions:
- when I want to see the stresses in the main beams in CS2 stage the program shows me the value 0 - you can see in the screenshot "STRESS CS2";
-  when I want to see the stresses in the main beams in CS4 stage the program shows me the value 0 - you can see in the screenshot "STRESS CS4";
I think that something is wrong because in CS2 and CS4 it is impossible to have value 0 for beams stresses.
Please verify that the diagrams  "My" in load combination "cLCB1" is ok or not. 

   
Hello dear Nandeep,

I understood what you explained me and I have managed to go ahead but I have another problem: I want to check for example pier elevation who is a circular section with diameter D=2.50 m from reinforced concrete. As you can see in the screenshot attached "01.ELEVATION CHECKING" I want to put the rebars on the circle perimeter but the maxim diameter of the rebars I can select id 18 mm(you can see in the same screenshot). I want to put rebars from 25 mm or 32 mm diameter, why is not possible to select diameters of rebars bigger than 18 mm? Another problem is expose screenshot 02 and 03, when I want to check the rebars the program give me next message: 
"Invalid rebars data for checking". Tell me please the mistake I have made on this step.
Thank you very much.
Best regards,




Hello dear Nandeep,

I want to determine the moments Mxx and Myy in the plinth, and the plinth is a plate. As you can see in the screenshot attached the local axis of the plates are not the same, just Z axis in fix but X and Y local exis are changing the direction on the plate elements and is a little bit  difficult to extract the values of the moments Mxx and Myy. My question is whether there is any way to rotate the axis that all the elements of the plinth to have the same direction of the X, Y and Z axis. How can I select only one element of the domain and see just for selected element the forces and the moments. The bridge model is attached in the last email I sent to you today.
Thank you very much and best regards again.



Hello dear Nandeep,

I apologize for many questions I ask, but the pressures are very high and I have to learn the program in very short time. This time I want to show me what I wrong in defining the seismic load like Response Spectrum function. You can see in the attaches screenshot the Response Spectrum function defining about Eurocode and the RS Load Case. When I want to perform analysis something is wrong and the program are stopping and does not give me any result. You can see that in the model attached. Best regards again.



Hello,

Sorry I couldn't get back to you yesterday.  Was sick after all that traveling and had to take a day off!
My response to each mail is as below:
1)  I have finished the stage construction and I understood all for this stage. Finally the program generated me a load combination
about Eurocode (I want to design the reinforced concrete about Eurocode) but I have next questions:
- when I want to see the stresses in the main beams in CS2 stage the program shows me the value 0 - you can see in the screenshot "STRESS CS2";
-  when I want to see the stresses in the main beams in CS4 stage the program shows me the value 0 - you can see in the screenshot "STRESS CS4";
I think that something is wrong because in CS2 and CS4 it is impossible to have value 0 for beams stresses.
A:  I believe you must have noticed as to why stress was 0.  For composite section, stress needs to be viewed by part.  Since model or screenshot weren't attached with this mail, I can't be sure of exact reason.  However, if this isn't resolved, let me know and I'll look into it.

2)  I want to check for example pier elevation who is a circular section with diameter D=2.50 m from reinforced concrete. As you can see in the screenshot attached "01.ELEVATION CHECKING" I want to put the rebars on the circle perimeter but the maxim diameter of the rebars I can select id 18 mm(you can see in the same screenshot). I want to put rebars from 25 mm or 32 mm diameter, why is not possible to select diameters of rebars bigger than 18 mm? Another problem is expose screenshot 02 and 03, when I want to check the rebars the program give me next message: "Invalid rebars data for checking". Tell me please the mistake I have made on this step.
A:  #18 is basically notation for american re-bars.  Kindly change the re-bar code from Tools> Preferences>Design/Load Code.

As for column checking, the Tie bar was not specified and that was the cause of the error.  Just the main bars were specified.

3)  I want to determine the moments Mxx and Myy in the plinth, and the plinth is a plate. As you can see in the screenshot attached the local axis of the plates are not the same, just Z axis in fix but X and Y local exis are changing the direction on the plate elements and is a little bit difficult to extract the values of the moments Mxx and Myy. My question is whether there is any way to rotate the axis that all the elements of the plinth to have the same direction of the X, Y and Z axis. How can I select only one element of the domain and see just for selected element the forces and the moments.
A:  It is possible to rotate the plate element axis, but that would be in pre-processing.  In this case, I'd rather recommend to check the results in global coordinate system.  That would resolve the problem of axis alignment.
Moreover, the rigid link connecting pier bottom to pile cap is not proper.  All the nodes of the pile cap which are inside the pier periphery should be the slave nodes.  To see result of any one element, simply activate only that element (Select and hit F2 on keyboard).

3)  This time I want to show me what I wrong in defining the seismic load like Response Spectrum function. You can see in the attaches screenshot the Response Spectrum function defining about Eurocode and the RS Load Case. When I want to perform analyse something is wrong and the program are stopping and does not give me any result. You can see that in the model attached.
A:  When going for analysis like response spectrum analysis, it is necessary to define mass and go for eigenvalue analysis, since RS analysis required time period, which in turn is obtained from eigenvalue analysis.
Above command converts load applied using Self Weight Command into mass.  Besides this, if any other load case is to be converted into mass, the Load> Static Loads> Loads to Masses feature has to be used.
To define eigenvalue analysis, simply go to Analysis> Eigenvalue and define the number of frequency as say 100.  The modified model is attached herewith for your review.
Kindly let us know if further assistance would be required.

Regards,
Nandeep
Technical Manager, MIDAS


Hello dear Nandeep,

Thank you very much for your responses that were great, I understood perfect but I have 3 more questions:
1) I have defined construction stages (CS1-CS4) and finally when I want to autogenerate the Load Combinations about Eurocode
(you can see first screenshot) in the autogenerated cLCB1 combination dead load appears in two positions, it means that dead load was
consider twice. of course that manually I can put from one of dead load 0 coefficient but it is possible that the program to generate
correctly the load combination? This think is strange for me...
2) I have defined the load Case "QUAKE" and I would like to see exactly the loads taken into account in this combination(QUAKE). Which of the load combination exposed in SCREENSHOT2 is the seismic one? Or is not exposed there and I need to see it from another menu?
Does the program automatically take into account the moving loads(masses from moving loads) or we have to introduce them automatically from Loads-Static Loads-Masses?
3) Please explain to me in your opinion how should the links between the plinth, bottom elevation of the pier and piles? If for example we will make the connections between bottom of the pier elevation, piles and plinth in the same horizontal plan located in the middle of the plinth thickness?
Thank you very much and best regards.


Hello,

The response to each issue are as below:
1) I have defined construction stages(CS1-CS4) and finally when I want to auto-generate the Load Combinations about Eurocode
(you can see first screenshot) in the auto-generated cLCB1 combination dead load appears in two positions, it means that dead load was
consider twice. of course that manually I can put from one of dead load 0 coefficient but it is possible that the program to generate
correctly the load combination? This think is strange for me...
A:  Kindly generate the combinations with CS Only setup as shown in the image below.  The static load cases of types which are not to be activated in construction stages (like temperature) would be automatically considered even with CS only option.
As you know, all the loads that are activated in construction stage are clubbed into Dead Load (CS) case.  If for some load case, the load factor is other than that of Dead Load, that particular load could be separated from Dead Load for CS using the construction stage analysis control.

2) I have defined the load Case "QUAKE" and I would like to see exactly the loads taken into account in this combination(QUAKE). Which of
the load combination exposed in SCREENSHOT2 is the seismic one? Or is not exposed there and I need to see it from another menu?
Does the program automatically take into account the moving loads(masses from moving loads) or we have to introduce them automatically from Loads-Static Loads-Masses?
A:  Seismic load is not automatically considered in the combination.  Kindly refer the image below from our online help manual.
Also, the live load mass has to be applied by the user.  To do this, the moving load tracer could be used to obtain the static position of the vehicle (Details) and then, this static load case could be converted into mass by using the load to mass feature.
Also, kindly refer our FAQs (Link) for any other doubt.

3) Please explain to me in your opinion how should the links between the plinth, bottom elevation of the pier and piles? If for example we will make the connections between bottom of the pier elevation, piles and plinth in the same horizontal plan located in the middle of the plinth thickness?
A:  In my view, all the nodes highlighted in the image below should be the slave node, since all of these would basically be in the joint region.
Kindly let us know if further assistance would be required.

Regards,
Nandeep
Technical Manager, MIDAS
POSTTENSIONED BRIDGE 1.mcb
DataImage20.png
POSTTENSIONED BRIDGE MODIFIED.mcb
01.MOVING LOAD OK.jpg
02.LOAD COMBINATION EUROCOD.jpg
POSTTENSIONED BRIDGE MODIFIED CS.mcb
DataImage32.png
POSTTENSIONED BRIDGE MODIFIED CS[1].mcb
CAPTURE 1 - CS.jpg
CAPTURE 2-CS.jpg
SCREEN 1.jpg
SCREEN 2.jpg
DataImage56[1].png
DataImage31.png
DataImage70.png
CS2.jpg
CS1.jpg
POSTTENSIONED BRIDGE MODIFIED CS.mcb
POSTTENSIONED BRIDGE 1.mcb
MOVING LOADS.jpg
DataImage28.png
DataImage26.png
DataImage51.png
DataImage56.png
DataImage46.png
POSTTENSIONED BRIDGE MODIFIED CS 2.zip
POSTTENSIONED BRIDGE MODIFIED CS 2.mcb
QUAKE.jpg
PLATE MOMENTS.jpg
POSTTENSIONED BRIDGE MODIFIED CS 1.mcb
02.ELEVATION CHECKING (2).jpg
03.ELEVATION CHECKING.jpg
01.ELEVATION CHECKING (3).jpg
DataImage85.png
DataImage11.png
POSTTENSIONED BRIDGE MODIFIED CS[1].mcb
PLATE .jpg
STR KM 14+199 -1.mcb
DataImage90.png
DataImage79.png
TAB 28 M.zip
TAB 28 M.mcb
TAB 28 M ANALYSE.mcb
POSTTENSIONED BRIDGE MODIFIED CS[2].mcb
CS2 DEFINED.jpg
Files
Sort by Name Sort by Date
CS2.jpg
270 KB
CS1.jpg
260 KB
QUAKE.jpg
367 KB
PLATE .jpg
355 KB
Get help for this page