Learning Forum

[vaibhavtaranekar]

Hello, i am trying to combine solid 185 with link180 using reinf264 elements but i come across an error everytime.

i am using following commands mentioned by @Wenlong 

 

finish

/prep7

! Define material properties

matid = 1001

mp,ex,matid,23827

mp,prxy,matid,.2

mp,dens,matid,.0001

! Define a new section id

sectypeid = 1002

secarea   = 10         !mm^2

! Define a new element type id

etype_id  = 1003

! Define a new section and new element type

sectype, sectypeid, reinf, discrete  ! Define a discrete reinf section

secdata, matid, secarea, mesh        ! Define the section properties

! Define a new element type Mesh200

et,etype_id,200,2

! Change the Link180 to Mesh200

esel,s,ename,,180

emodify, all, type, etype_id        ! Define a  

emodify, all, secnum, sectypeid

! Select both the Mesh200 and the base Solid185 element

esel,all

! Generate reinf264 elements. 

EREINF

! Delete the mesh200 elements

esel,s,ename,,mesh200

edele,all

FINISH

! To verify, we can print the the element types

allsel,all

/com,============================================

etlist,all

/com,============================================

/com, =====  Solid elements =========

esel,s,ename,, 185

/com, =====  Link elements =========

esel,s,ename,,180

/com, =====  Reinforce element =========

esel,s,ename,,264

allsel,all 

! Go to solution module

/SOLU

 

I getting following error in solution information.

 *** ERROR ***                           CP =       0.609   TIME= 137:46
 No base element is found for reinforcing Element 3073.  Use of isolated
 reinforcing elements is not permitted

Kindly provide remedy for this issue. 

 

Thanks!

[gigihmprayogo]

Hi, did you already solve the problem?i have same problem, but my error message said: "no new reinforcing element was generated etc"

[vaibhavtaranekar]

no, i havn't been succesful in able to use reinf264 elements. can you share your commands? i would like to see if there is something i can fix.

[gigihmprayogo]

I used same snippet from @Wenlong, for reinforced concrete instead of using REINF command, I am using coupled degrees of freedom between coincident nodes (CPINTF), but you must set and mesh element between solid and link/beam element until it has coincident nodes, create group named selection for solid and link/beam element after that u can used these command

[Wenlong]

Hi vaibhavtaranekar,

Can you highlight the element 3073 and see where it is located? Maybe share a screenshot?

Regards,

Wenlong

 

[Wenlong]

Hi vaibhavtaranekar,

I understand the frustration you have experienced. The thing is when your model gets complicated with complex geometry and nonlinear materials, it becomes hard to find the root cause of the problem. I also went through a lot of iterations to get the command snippet work. What I did to debug is, I created a two-element model (one for concrete, one for rebar inside the concrete). It greatly simplifies the process and makes the logic much clearer. Once you are successful with that small model, you can migrate to your large model. Of course, I am also happy to help.

Regards,

Wenlong

 

 

 

[Wenlong]

Hi gigihmprayogo,

Thanks for sharing the experience with CPINTF commands. One question is, how to make sure the rebars and the concrete have the coincident nodes? Is that achieved by partitioning the geometry?

Regards,

Wenlong

 

[vaibhavtaranekar]

i have also been using following commands to make the simulation run. 

/PREP7

ESEL,S,ENAME,,65

ESEL,A,ENAME,,180

ALLSEL,BELOW,ELEM

CEINTF,0.001,

ALLSEL,ALL

/SOLU

OUTRES,ALL,ALL

 

[vaibhavtaranekar]

what i usually do is set the rebars at fixed spacing of the mesh i am going to set, for example i set rebars at 50mm from edge then i use 50mm mesh to have coinciding nodes. I am soon going to try your EREINF commands as soon as i am free, and let yo know if there's any success.

[gigihmprayogo]

I'm not partitioning the geometry, i'm just design the model in CAD first, so basically I plan the geometry and mesh size there, then i go to the Design Modeler & Mechanical module to make the geometry and mesh size of the model are exactly same from what I made before..It is need extra effort, but that's the only way I can do it. I want to compared with REINF264, but its just not yet working

[vaibhavtaranekar]

i am trying to use REINF264, will let you know if i succeed. 

[Wenlong]

Hi gigihmprayogo,

When you use EREINF, what error message you are seeing? Here is another example about EREINF and concrete: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v193/ans_tec/tecreinfconc.html

Regards,

Wenlong

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image


• How to use Google to search within Ansys Student Community

 

 

[vaibhavtaranekar]

@gigihmprayogo I was able to run my model using the commands provided by @Wenlong in the post https://forum.ansys.com/forums/topic/cyclic-loading-8/ . I have not tested the differences and benefits of using REINF264 over CEINTF/CPINTF commands. However the model ran succesfully and i was able to visualize the model with reinforcement.

Thanks to Wenlong for the help.

Best of luck

[gigihmprayogo]

@Wenlong,

Here the error message

If i selected for link element only for reinforcing, it succesfully generated REINF (shown below).It seems REINF264 has reinforcing link element instead of solid element (concrete), I have run these model and it seems REINF264 do not reinforced solid element..please advice

[gigihmprayogo]

@vaibhavtaranekar, could you please share your the latest snippet and explain your step to build your model.

[vaibhavtaranekar]

firstly select your concrete and rebar bodies and add named selection seperately for "concrete" and "rebars". then add the line "steel_mat_id=matid" in your line bodies. Add the command mentioned below for REINF264 and you can post process it to view the model.

ADPL for line bodies:

*get,myarea,SECP,matid,PROP,AREA ! gets the area and  assigns it to myarea

 

ET,matid,LINK180 ! define link element

steel_mat_id=matid

SECTYPE,matid,LINK ! assign link

 

SECDATA,myarea ! assign area

 

MPDATA,EX,matid,,2e5

 

MPDATA,PRXY,matid,,0.3  

 

TB,BISO,matid,1,2,

 

TBDATA,,400,0

ADPL for REINF264

finish

/prep7

 

!

---

!

!   Get the maximum element type id and section id

!

!

---

*get, typid, elem, 0, typm 

*get, secid, secp, 0, num, max

 

sectypeid = secid + 1   ! Create a new section id by shifting the max by 1

etype_id = typid + 1    ! Create a new type id by shifting the max by 1     

 

!

---

!

!   Define the reinforcement section type and Mesh200 element type

!

!

---

 

secarea = 113.10  ! Define a section area for the reinforcement

 

sectype, sectypeid, reinf, discrete         ! Define a discrete reinf section

secdata, steel_mat_id, secarea, mesh        ! Define the section properties

 

et, etype_id, 200, 2    ! Define a new element type

 

!

---

!

!   Generate Mesh200 elements 

!

!

---

 

cmsel, s, rebars, elem  ! Select the name selection "rebars". 

                        ! The name selection has to be bodies instead of edges

emodify, all, type, etype_id        ! Change the element type to Mesh200

emodify, all, secnum, sectypeid     ! Change the section to discrete reinf

 

!

---

!

!   Generate Reinf264 elements based on Mesh200 and solid elements

!

!

---

 

cmsel, a, concrete, elem            ! Add concrete to the selection                  

EREINF                              ! Generate reinforcement elements

 

esel,s,ename,,mesh200               ! Select the Mesh200 elements

edele,all                           ! Delete the Mesh200 elements

FINISH

 

allsel,all 

/SOLU

OUTRES,ALL,all 

To View the results in post processing

! $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$4

 

! Graphics power needs to be turned on to view the rebars

 

/graphics,power

! Enter /post1 module

/post1

! Show result as a png image

/SHOW,png

! Set the frame as the last substep of the 1st step

 

set,1,last

 

! Select the SOLID185 elements

 

esel,s,ename,185

 

/trlcy,elem,0.5     ! Change them to transparent level 0.5 (0 is solid, 1 is completely transparent)

esel,all

! Set view angle

 

/view,1,1,1,1

 

/angle,1,-0.75

! Show the whole section of the reinforcement

/eshape,1 

! Plot displacement

plnsol,u,x 

! $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$

I hope it works for you. We still have to figure out how to use REINF if there are multiple different sized rebars in the model.

 

[gigihmprayogo]

Finally i found the source of error, its because i'm using CPT215 as base element, when i change base element to SOLID185 for example, the snippet works..So if you are modelling concrete using coupled damage-plasticity microplane model with CPT215, set base element with SOLID185 first then use snippet above from @Wenlong, after command line delete mesh200, add another line to change SOLID185 to CPT215

[Wenlong]

Hi gigihmprayogo,

Great! Thanks for the feedback!

Regards,

Wenlong

 

[vaibhavtaranekar]

Finally i found the source of error, its because i'm using CPT215 as base element, when i change base element to SOLID185 for example, the snippet works..So if you are modelling concrete using coupled damage-plasticity microplane model with CPT215, set base element with SOLID185 first then use snippet above from @Wenlong, after command line delete mesh200, add another line to change SOLID185 to CPT215

Kindly post the new snippets you used for CPT215, or just the commmand used to modify the SOLID185 to CPT215.

[gigihmprayogo]

First, you need to create body selection group for all body that you want to define and assign. Here are my example /PREP7 snippet:

 

/PREP7

 

ALLSEL,ALL

 

! Element Type Identification

*GET,ETID,ELEM,0,TYPM

CONCRETE_ET_ID = ETID + 1

STEEL_ET_ID = ETID + 2

MESH200_ET_ID = ETID + 3

CONCRETE_TEMP_ET_ID = ETID + 4

 

! Material Model Identification

*GET,MATID,ELEM,0,MATM

CONCRETE_MAT_ID = MATID + 1

REBARSD10_MAT_ID = MATID + 2

REBARSD13_MAT_ID = MATID + 3

REBARSD19_MAT_ID = MATID + 4

REBARSD25_MAT_ID = MATID + 5

STEEL_MAT_ID = MATID + 6

 

! Section Type Identification

*GET,SECID,SECP,0,NUM,MAX

D10_SEC_ID = SECID + 1

D13_SEC_ID = SECID + 2

D19_SEC_ID = SECID + 3

D25_SEC_ID = SECID + 4

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! Section 1: Define Element Type !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

! #1 Concrete

ET,CONCRETE_ET_ID,CPT215 ! Define elements as CPT215

KEYOPT,CONCRETE_ET_ID,18,2     ! Activate extra degrees of freedom

 

! #2 Steel

ET,STEEL_ET_ID,SOLID185            ! Define elements as SOLID185

 

! #3 MESH200

ET,MESH200_ET_ID,MESH200,2

 

! #4 Temporary Concrete

ET,CONCRETE_TEMP_ET_ID,SOLID185

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! End of Section 1 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

 

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! Section 2: Define Material Property !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

! #1 Concrete

! Material Model --> Concrete: Coupled Damage-Plasticity Microplane

Ec = 32200

Nuc = 0.2

Densc = 2.4e-06

fuc = 54.8 

fbc = 63.02

fut = 3

Rt = 4    

D_ = 2e4

sigVc = -45  

R_ = 2   

c = 2500    

m_ = 5  

gamt0 = 0 

gamc0 = 0.00068 

betat = 3000

betac = 2000

! Define Elastic Properties of Material Concrete

MP,EX,CONCRETE_MAT_ID,Ec     ! Define Elasticity Modulus

MP,NUXY,CONCRETE_MAT_ID,Nuc         ! Define Poisson's ratio     

MP,DENS,CONCRETE_MAT_ID,Densc     ! Define material Density

! Define Coupled Damage-Plasticity Microplane Properties

TB,MPLANE,CONCRETE_MAT_ID,,,DPC

TBDATA,1,fuc,fbc,fut,Rt,D_,sigVc

TBDATA,7,R_,gamt0,gamc0,betat,betac

TB,MPLA,CONCRETE_MAT_ID,,,NLOCAL

TBDATA,1,c,m_

 

! #2 Rebars

Densr = 7.85e-6

Er = 2e5

Nur = 0.3

fy_D10 = 400

fy_D13 = 400

fy_D19 = 500

fy_D25 = 400

tanmodr = 1000

 

! Define Elastic Properties of Material Rebars D10

MP,DENS,REBARSD10_MAT_ID,Densr

MP,EX,REBARSD10_MAT_ID,Er

MP,NUXY,REBARSD10_MAT_ID,Nur

! Define Bilinear Isotropic Hardening D10

TB,PLAS,REBARSD10_MAT_ID,2,,BISO

TBTEMP,0

TBDATA,1,fy_D10,tanmodr

 

! Define Elastic Properties of Material Rebars D13

MP,DENS,REBARSD13_MAT_ID,Densr

MP,EX,REBARSD13_MAT_ID,Er

MP,NUXY,REBARSD13_MAT_ID,Nur

! Define Bilinear Isotropic Hardening D10

TB,PLAS,REBARSD13_MAT_ID,2,,BISO

TBTEMP,0

TBDATA,1,fy_D13,tanmodr

 

! Define Elastic Properties of Material Rebars D19

MP,DENS,REBARSD19_MAT_ID,Densr

MP,EX,REBARSD19_MAT_ID,Er

MP,NUXY,REBARSD19_MAT_ID,Nur

! Define Bilinear Isotropic Hardening D10

TB,PLAS,REBARSD19_MAT_ID,2,,BISO

TBTEMP,0

TBDATA,1,fy_D19,tanmodr

 

! Define Elastic Properties of Material Rebars D25

MP,DENS,REBARSD25_MAT_ID,Densr

MP,EX,REBARSD25_MAT_ID,Er

MP,NUXY,REBARSD25_MAT_ID,Nur

! Define Bilinear Isotropic Hardening D10

TB,PLAS,REBARSD25_MAT_ID,2,,BISO

TBTEMP,0

TBDATA,1,fy_D25,tanmodr

 

! #3 Steel

Denss = 7.85e-6

Es = 2e5

Nus = 0.3

fys = 1000

tanmods = 1000

! Define Elastic Properties of Material Rebars

MP,DENS,STEEL_MAT_ID,Denss

MP,EX,STEEL_MAT_ID,Es

MP,NUXY,STEEL_MAT_ID,Nus

! Define Bilinear Isotropic Hardening

TB,PLAS,STEEL_MAT_ID,2,,BISO

TBTEMP,0

TBDATA,1,fys,tanmods

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! End of Section 2 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

 

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! Section 3: Define Section Type !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

A_D10 = 78.5

A_D13 = 129.0

A_D19 = 283.0

A_D25 = 490.0

 

! Define Reinforcement Section D10

SECTYPE,D10_SEC_ID,REINF,DISCRETE           ! Define a discrete reinf section

SECDATA,REBARSD10_MAT_ID,A_D10,MESH         ! Define the section properties

 

! Define Reinforcement Section D13

SECTYPE,D13_SEC_ID,REINF,DISCRETE           ! Define a discrete reinf section

SECDATA,REBARSD13_MAT_ID,A_D13,MESH         ! Define the section properties

 

! Define Reinforcement Section D19

SECTYPE,D19_SEC_ID,REINF,DISCRETE           ! Define a discrete reinf section

SECDATA,REBARSD19_MAT_ID,A_D19,MESH         ! Define the section properties

 

! Define Reinforcement Section D25

SECTYPE,D25_SEC_ID,REINF,DISCRETE           ! Define a discrete reinf section

SECDATA,REBARSD25_MAT_ID,A_D25,MESH         ! Define the section properties

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! End of Section 3 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

 

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! Section 4: Assign Element, Material & Section !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

! #1 Assign Concrete Element Type to Temporary Element

CMSEL,S,CONCRETE,ELEM

EMODIF,ALL,TYPE,CONCRETE_TEMP_ET_ID

 

! #2.1 Assign Rebars D10 Using REINF264

CMSEL,S,D10,ELEM

EMODIF,ALL,TYPE,MESH200_ET_ID       ! Change the element type to Mesh200

EMODIF,ALL,SECNUM,D10_SEC_ID        ! Change the section to discrete reinf

 

! #2.2 Assign Rebars D13 Using REINF264

CMSEL,S,D13,ELEM

EMODIF,ALL,TYPE,MESH200_ET_ID       ! Change the element type to Mesh200

EMODIF,ALL,SECNUM,D13_SEC_ID        ! Change the section to discrete reinf

 

! #2.3 Assign Rebars D19 Using REINF264

CMSEL,S,D19,ELEM

EMODIF,ALL,TYPE,MESH200_ET_ID       ! Change the element type to Mesh200

EMODIF,ALL,SECNUM,D19_SEC_ID        ! Change the section to discrete reinf

 

! #2.4 Assign Rebars D25 Using REINF264

CMSEL,S,D25,ELEM

EMODIF,ALL,TYPE,MESH200_ET_ID       ! Change the element type to Mesh200

EMODIF,ALL,SECNUM,D25_SEC_ID        ! Change the section to discrete reinf

 

! Generate Reinforcing Element

CMSEL,S,CONCRETE,ELEM               ! Select Concrete Element

CMSEL,A,REBARS,ELEM                 ! Add All Rebar Element to Selection

EREINF                              ! Generate reinforcement elements

 

ESEL,S,ENAME,,MESH200               ! Select the Mesh200 elements

EDELE,ALL                           ! Delete the Mesh200 elements

 

! Change Concrete from Temporary Element to CPT215

CMSEL,S,CONCRETE,ELEM

EMODIF,ALL,TYPE,CONCRETE_ET_ID

EMODIF,ALL,MAT,CONCRETE_MAT_ID

 

! #3 Steel 

CMSEL,S,STEEL,ELEM

EMODIF,ALL,TYPE,STEEL_ET_ID

EMODIF,ALL,MAT,STEEL_MAT_ID

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! End of Section 4 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

 

ALLSEL,ALL

/SOLU

[vaibhavtaranekar]

Thank you so much for the commands. Can you upload your archive file so that i can better understand how you used REINF for different bars of steel? I am having problem with that. 

Did you put any commands for concrete and line bodies or have you directly put the commands in preprocessing?

[gigihmprayogo]

Sure, please give me your email.

I did not put any command on line or solid body, just put all command on pre processing

[Youssef Abbas]

Hi, 

can you send me the archive file to to understand how you used REINF for different bars of steel.

Youssef.abbas@gmx.net

[vaibhavtaranekar]

my email id is vaibhavtaranekar1@gmail.com 

Thank you in advance

[rickywugunawan]

Hi, can I also ask for your file? right now I'm also modelling a RC beam-column joint and I faced some problems.nnThank you very muchnnBest Regards,nRickyn

[rickywugunawan]

Hi Array. Thanks for the informationnI try to follow your following suggestion on a simple RC beamnfirstly select your concrete and rebar bodies and add named selection seperately for concrete and rebars. then add the line steel_mat_id=matid in your line bodies. Add the command mentioned below for REINF264 and you can post process it to view the model.nHowever, it seems that the rebar and the concrete is not connected as it is shown in the picture. Does this also happen to you?nAlso, how do you input the concrete strength? nBelow, I also attached my model with the model name REINF264 inside. Hopefully you can take a look. nThank you so muchnRegards, nRickynArraynn

[O_Maxwell]

Hi, have been following your success with the subject . Am also curious to know how you defined, assigned and input your command snippet on pre processioning. Am currently working on simulating a reinforced concrete Bridge deck under cyclic loading condition. please can you share your file?.Edit Admin. Please share files on here so everyone can benefit. n

[Erik Kostson]

We have a great workflow in our latest release (2020 R2) where we do not need to use any commands anymore for the reinforcements. Just in the cross section under details of the line body, instead of beam choose reinforcement (see image below, yellow marking).Also for the concrete we recommend using Menetrey-Willam (MW model) as this has been tested/benchmarked against tests, and shown to predict different types of failure in RC structure fairly well. Again you can define the MW properties in engineering data so no snippets are needed anymore. So it is now much easier to model even complex RC structure and without using snippets.nnn

[a.m.aanikce]

Can you share the file with me?n

[Erik Kostson]

As we discussed in a previous , use the current 2020 r2 workflow for reinforcements and the MW material like you say you do in your other comment . This is because using snippets can cause a lot of issues, and give wrong results if not properly checked - so use the 2020 r2 as shown below (also post processing is difficult for the reinf using snippets):nIn 2020 r2 for reinf: in the cross section under details of the line body, instead of beam choose reinforcement (see image below, yellow marking). MW is defined in engineering data.nn

[O_Maxwell]

Hi, nThis is great news to know. But please still need clarification with the following:nMaterial Properties are defined from the Engineering Data right? (If using Work Bench)n Can My rebars be defined as solid bodies too ? (alternatively)nAny need to ensure coinciding nodes between the rebars and the concrete?nThanks a million for your anticipated response.n