Ansys workbench Composite Analysis

  • #1
Hello All,

I am a master student working on my thesis. am using ANSYS workbench to model the debonding between FRP and Concrete (Single Shear Test). The geometry is very simple, so meshing and sketching were easy. however I have the following quires about loading and interfaces.
1. I want to apply a displacement controlled load ( at a rate of 2mm/min) to be exact, ANSYS provide you with three Load choices (Constant, Tabular or Function), How can I apply this load rate with these choices. do I have to play with the number of steps, initial, minimum, and maximum time step to apply this type of loading.
2. For this type of modeling (composites modeling) there are two methods to apply (Cohesive Zone Model "CZM" or Virtual Crack Closure Technique "VCCT"). these two methods need a surface/interface to be applied on. in my model I used CZM which is easy to apply, but on which surface/interface (FRP/Adhesive or Adhesive/concrete) interface. or within the adhesive layer it self by slicing it into two parts.
Capture.JPG

3. For the other Surfaces (contacts pairs), ANSYS automatically generates a bonded contact by default. is this the contact type I should use with my analysis, bearing in mind that in reality separation could occur in any interface (FRP/Adhesive or Adhesive/concrete).

Any help or suggestions will be highly appreciated.
Thanks in advance
 

Answers and Replies

  • #2
9
4
Hello.

1. So, yo want to apply velocity 2mm / min by means of displacement control. Let's say your end time is 1s. Given that displacement = velocity * time, it should not be a problem to find what displacement you need to apply. Or, if you have given displacement you need to solve for, then find appropriate end time.

2. I never modeled composites, so I am not a best person for this, but looking at your picture, I would probably delete adhesive layer and apply bonded contact between basic materials. Then you can specify a debonding condition for this contact. Knowing maximum load your adhesive layer can withstand, you can tune debonding condition accordingly. Just type "debonding" into workbench help, you should get some hints.

3. See 2.
 
  • #3
Hello.

1. So, yo want to apply velocity 2mm / min by means of displacement control. Let's say your end time is 1s. Given that displacement = velocity * time, it should not be a problem to find what displacement you need to apply. Or, if you have given displacement you need to solve for, then find appropriate end time.

2. I never modeled composites, so I am not a best person for this, but looking at your picture, I would probably delete adhesive layer and apply bonded contact between basic materials. Then you can specify a debonding condition for this contact. Knowing maximum load your adhesive layer can withstand, you can tune debonding condition accordingly. Just type "debonding" into workbench help, you should get some hints.

3. See 2.
Thank you for your reply Gobi. Really appreciate it.

I went through some articles and I reached the same point you said, that I should delete the epoxy layer and apply the CZM method (or any contact condition) on the contact region between the plate and the concrete, then I can implement the adhesive properties in it. this way I can model the debonding between these two materials.

Regarding your 1st point. I conducted the experimental program with a UTM machine. the load applied by the machine on the specimen was 2mm/min " Till the spacemen Failure". as you said, given the step end time and the load rate (2mm/min) I can find the displacement. however experimentally I loaded the specimen "till failure". my question is (if I applied the displacement calculated from the equation (displacement = velocity * time) based on the end time and the velocity, will the specimen fail, I tried it already and I think you are right (the result are still not close to experimental though), but I think this is due to contact, I have to work more on it).

Thank you again for your useful points.
Best regards
 
Last edited:
  • #4
9
4
I am not sure I understood your question correctly (English is not my native language), but I will try :

If you loaded "till failure", there should be corresponding displacement in UTM output. So, instead of calculating displacement from end time and speed, you need to calculate step end time based on your experimental data. I would probably set a little longer time than calculated, just to be sure. After that, if still no failure is occuring in the simulation, problem is somwhere else (possibly contact, as you mentioned).
 
  • #5
hi every one I am modeling the debonding between concrete and CFRP subjected to tangential loading I used the contact element with CZM model now my problem is that the experimental and the analytical curves are different I want to ask what are the value of FKN and FKT that you used and what are the keyoptions and what about the real constant for contact element that I should use to overcome this problem?
 
  • #6
Which ANSYS version you are using?? is it Workbench or APDL. I also didn't fully understand your model and how is the force applied. I am working with workbench (I didn't use APDL before) and am still working on composites debonding problems. if you are working with workbench, my advice to you is to start step by step. by that I mean first
1. you have to solve the model linearly with out the CZM, assuming that the two contact surfaces (CFRP/ Concrete) are fully bonded. apply any tangential loading solve it by hand and then compare the two answers. you have to make sure that the materials properties in the engineering data are accurate
2. in some cases you have to insert APDl commands in the workbench model tree
Solid 65 for concrete
Link 180 for reinforcement (if you have steel)
Solid 63 for FRP.
3. After that apply the CZM or VCCT method. (if you conduct the experimental insert the values you obtained from that in your model for the CZM or the VCCT methods) in engineering data (Fracture energy based / seperation distance based/ interface delamination (bilinear or exponential))
Check the paper attached for CZM engineering data. also check this videos links:
In general
FKN = 10 for bonded.
For all other, FKN = 1.0
but if bonded and other contact behavior exists, FKN = 1 for all

Best of luck
 

Attachments

  • CZM .pdf
    284.6 KB · Views: 5,631
  • #7
thanks for your answering, I am using ANSY APDL, I used plane 183 to represent concrete and CFRP , target169 and cont172 with CZM to model the interface between the concrete and CFRP, since the model is subjected to tangential load (mode 2) I used the parameters c3,c4,c5 only and I used Xinzheng Lu to calculate these parameter. how did you calculate your parameter? . I tried to use 3D model the same think the experimental and the analytical models are too different. in the attached pdf and photographs the model that I am trying to model and the model I used to calculate the czm parameters. wishing to hear your opinion.
 

Attachments

  • Lu_et_al_2005.pdf
    2.8 MB · Views: 555
  • ansys.png
    ansys.png
    32.8 KB · Views: 1,255
  • ansys1.png
    ansys1.png
    38.6 KB · Views: 961
  • #8
I am using ANSYS Workbench because the user interface is much easier than APDL. I don't have experience with APDL. but the parameters are directly depend on the experimental results (if you did some experimental). from the experimental data draw the (Bond Stress - Slip) curve and obtain the parameters C3, C4, C5 (mode II) based on models with approximately the same general trend, see the attached images for how to obtain the parameters. If you didn't conduct any experimental work then for sure you are trying to fit the curve based on some given data or previous paper, then see in that paper how they obtained these parameters (equations/models) and calculate the parameters from there. in case this didn't work then check one by one
1.materials properties (CFRP-Concrete-Epoxy)
2. Element Types
3.Contact

Parameters.PNG
Experimental .PNG

Parameters from bond slip.PNG
Parameters.PNG
Workbench parameters.PNG


Best of Luck
 

Attachments

  • Parameters 2.PNG
    Parameters 2.PNG
    7.8 KB · Views: 1,021
Last edited:
  • #9
2
0
Hi Everyone,

I tried to enter the above relationship as command in Ansys Workbench, but it didn't effect the results at all. I entered the command in static structural section as below. Please advice if you tried it before or there is something wrong in the command. (I used the value of the above example in the command just as an example)

TB,CZM,1,2,,CBDD
TBDATA,1,1.7,0.06,2,0.03,0.000001,1

upload_2016-9-22_10-30-48.png

upload_2016-9-22_10-30-5.png
 

Attachments

  • upload_2016-9-22_10-30-26.png
    upload_2016-9-22_10-30-26.png
    29 KB · Views: 932
  • upload_2016-9-22_10-30-34.png
    upload_2016-9-22_10-30-34.png
    29 KB · Views: 783
  • #10
hello, I don't know why do you want to use a command block for defining the CZM material in workbench, you can do exactly as the previous example you mentioned. just define a new material in engineering data and enter the parameter values. check the 1st video on top. its very helpful.
 
  • #11
2
0
Thanks, Ahmed.

I tried as you said earliar but it is giving me very small values which is not close to the experimental results at all.
 
  • #12
Can you define your problem?. what type of analysis you are doing??. did you conduct any experimental testing to compare your model with??
 
  • #13
Hi,

Does the ANSYS WB 13 support ACP or any kind of composite
Hello All,

I am a master student working on my thesis. am using ANSYS workbench to model the debonding between FRP and Concrete (Single Shear Test). The geometry is very simple, so meshing and sketching were easy. however I have the following quires about loading and interfaces.
1. I want to apply a displacement controlled load ( at a rate of 2mm/min) to be exact, ANSYS provide you with three Load choices (Constant, Tabular or Function), How can I apply this load rate with these choices. do I have to play with the number of steps, initial, minimum, and maximum time step to apply this type of loading.
2. For this type of modeling (composites modeling) there are two methods to apply (Cohesive Zone Model "CZM" or Virtual Crack Closure Technique "VCCT"). these two methods need a surface/interface to be applied on. in my model I used CZM which is easy to apply, but on which surface/interface (FRP/Adhesive or Adhesive/concrete) interface. or within the adhesive layer it self by slicing it into two parts.
View attachment 97248
3. For the other Surfaces (contacts pairs), ANSYS automatically generates a bonded contact by default. is this the contact type I should use with my analysis, bearing in mind that in reality separation could occur in any interface (FRP/Adhesive or Adhesive/concrete).

Any help or suggestions will be highly appreciated.
Thanks in advance


Hi,
Sorry, I am posting in the wrong area, but can you please help me one thing.
Do we have ACP in ANSYS WB13 ? Is there any method where we can do a composite analysis in ANSYS WB 13?
Thanks in advance.
 
  • #14
Hello,

What I know is that when you download any version of ANSYS. it's like a package including all (Fluent, APDL, WB, ACP, AIM, AQWA...etc). if you have a layered composite, in this case you may need to use ACP, but for single plate/sheet you can use WB.
 
  • #15
Thanks a lot Ahmad.
I understand, but in in my WB, there is no option for ACP, whereas I have installed the entire package of ANSYS 13, that is why I was wondering that if the ANSYS 13 package support ACP or not.
 
  • #16
Hi Ahmed,

How do you know the material behavior parameters for CZM?
like (TBDATA,1,1.7,0.06,2,0.03,0.000001,1) in #9
 
  • #17
hellow jeff,

if you look at #8 above you will see the graph relating the bond stress vs slip with the parameters defined (the graph in red), the excel graph above it (in blue) is generated using an equation depending on experimental strain gauge readings. if you did the exact same test with strain gauges then you can draw the bond-slip curve. if you did other tests on beams..etc, then you can use one of the bond-slip models available in the literature.
 
  • #18
Thank you very much, Ahmed.
One more question.
How do you know the CZM elements start to break? compare the fracture energy with the critical fracture energy or something else?
In other words, what is the failure criteria of CZM elements?

Thank you again.
 
  • #19
Hi Jeff,

you can do that if you used fracture based debonding. if you choose separation based debonding then you can do the following:
based on your simulation results. on the solution branch you can insert a contact tool and enter the following:
Frictional stress: the max value should be approximately as same value as the one entered in engineering data for the "maximum tangential contact stress".
Sliding Distance: the max value should be approximately as same value as the one entered in engineering data for the "tangential slip at completion of deonding".
other thing you can do is to turn animation on and see it actually debond "slide at the end of the animation"..
 
  • #20
I will try. Thank you so much for your reply, Ahmed.:smile:
 
  • #21
6
0
I am using ANSYS Workbench because the user interface is much easier than APDL. I don't have experience with APDL. but the parameters are directly depend on the experimental results (if you did some experimental). from the experimental data draw the (Bond Stress - Slip) curve and obtain the parameters C3, C4, C5 (mode II) based on models with approximately the same general trend, see the attached images for how to obtain the parameters. If you didn't conduct any experimental work then for sure you are trying to fit the curve based on some given data or previous paper, then see in that paper how they obtained these parameters (equations/models) and calculate the parameters from there. in case this didn't work then check one by one
1.materials properties (CFRP-Concrete-Epoxy)
2. Element Types
3.Contact

View attachment 101278 View attachment 101279
View attachment 101280View attachment 101278 View attachment 101281

Best of Luck

May be by this time you have already solved the problem. I am trying to simulate the same in Ansys workbench. Could you kindly guide me how did you solve the problem stated in your first post of this thread? I also applied the controlled displacement until specimen failure. I assume you applied velocity on in the simulation and calculated the end time based on the displacement value (from the experiment). Could you please confirm that you did like this or something different?

Which CZM model did you use in your simulation? (Bilinear, Separation, Fracture or Exponential)? In my model I cant seem to apply the exponential and Bilinear. Cant figure out why.

Did you only use one model/simulation only or you made separate models like one for till the elastic region, then second for the debonding and then to model the non-linear behavior?

If you do not mind, Is it possible to share the model which you made to simulate the debonding in ansys workbench?

Thank you
 
  • #22
6
0
Thanks, Ahmed.

I tried as you said earliar but it is giving me very small values which is not close to the experimental results at all.

Eng Abla, I suppose you might have already solved the problem. Could you please share how did you solved the problem of getting small values in FEA as compared to the experimental results?
 
  • #23
3
0
Hello All,

I am a master student working on my thesis. am using ANSYS workbench to model the debonding between FRP and Concrete (Single Shear Test). The geometry is very simple, so meshing and sketching were easy. however I have the following quires about loading and interfaces.

1. I want to apply a displacement controlled load ( at a rate of 2mm/min) to be exact, ANSYS provide you with three Load choices (Constant, Tabular or Function), How can I apply this load rate with these choices. do I have to play with the number of steps, initial, minimum, and maximum time step to apply this type of loading.

2. For this type of modeling (composites modeling) there are two methods to apply (Cohesive Zone Model "CZM" or Virtual Crack Closure Technique "VCCT"). these two methods need a surface/interface to be applied on. in my model I used CZM which is easy to apply, but on which surface/interface (FRP/Adhesive or Adhesive/concrete) interface. or within the adhesive layer it self by slicing it into two parts.
View attachment 97248

3. For the other Surfaces (contacts pairs), ANSYS automatically generates a bonded contact by default. is this the contact type I should use with my analysis, bearing in mind that in reality separation could occur in any interface (FRP/Adhesive or Adhesive/concrete).

Any help or suggestions will be highly appreciated.
Thanks in advance

Please does Ansys generate one of the contact pairs e.g ADHESIVE/CONCRETE while I use CZM for the other contact e.g FRP/ADHESIVE?
 

Related Threads on Ansys workbench Composite Analysis

  • Last Post
Replies
0
Views
1K
Replies
1
Views
4K
  • Last Post
Replies
2
Views
2K
  • Last Post
Replies
1
Views
3K
  • Last Post
Replies
1
Views
223
Replies
3
Views
4K
Replies
1
Views
1K
Replies
0
Views
1K
Replies
1
Views
2K
Replies
8
Views
10K
Top