# SIMULATION OF COMPRESSION TEST IN ANSYS

• 265 Views
• Last Post 2 days ago
• Topic Is Solved
saurabhiitk posted this 19 February 2020

Dear friends

My task is to simulate a compression test on ANSYS. The material of the specimen is ABS(ACRYLONITRILE BUTADIENE STYRENE). The deformation velocity to be used is 25mm/min. Right now i am using transient structural for the same.

What are the steps that i should take to achieve my desired result?

peteroznewman posted this 19 February 2020

Don't use Transient Structural.

Use Static Structural, and use a Displacement Boundary Condition.

What shape is the sample? Is it a cylinder?  If so, use an axisymmetric 2D model.

If it has 3 planes of symmetry, cut through the center of the sample on those 3 planes and use Symmetry BCs to simplify the model.

What kind of material model do you have?  You must have plasticity in the model if you want to test past the elastic region.

saurabhiitk posted this 19 February 2020

sir

•  the specimen that i am using for the compression test has been attached below.  I am using multilinear kinematic hardening model for plasticity. please suggest the steps that i should take to get stress strain curve for both elastic and plastic region. Generally i get linear stress strain curve even if the equivalent stress value exceeds the yield strength value.
• also please suggest the steps that i should take to simulate the compression tests in static structural.(as mentioned by you in your post).

• Liked by
peteroznewman posted this 19 February 2020

You have the stress-strain curve for the material.  That material has been formed into a shape, and now you want to simulate the force-displacement curve that results from compressing that structure.  What direction is is being compressed, X or Y or Z?  How is it supported?

It has 3 planes of symmetry, so cut through the center of the sample on those 3 planes and use Symmetry BCs to simplify the model.

You might have to compress it a long way before the force-displacement curve deviates from a straight line.  How much compression do you need to test it to?  If the initial sample length is 25, what is the final length when you stop the test?

saurabhiitk posted this 20 February 2020

1) i am using fixed support at one end. i am trying to apply velocity in only one direction( in this case z direction).

2) i have stress-strain data obtained from compression test results that i have already done in my lab.

3) i have used multiple deformation speed for compressing the specimen. ( values are 1.35,1.5 4.5, 13.5, 25(mm/min))

4) i have done compression till whole material has collapsed. (i.e. till the time when the hexagonal hole( cell) present in the specimen is closed and complete crushing of the specimen takes place.

5) the time till  which  compression is done is dependent on deformation velocity( higher the deformation velocity lesser the time taken for compression).

6) please till me about the basic process to follow to simulate this test in ANSYS. I am unable to understand your concept of plane of symmetry. HOW TO DO IT?

7) should i use the data of true stress- strain curve?

8) please also suggest the steps that i should take to get the load-displacement , stress- strain curve which should match the curve that i get from compression test. what are the required settings to be done to get these curves.

i know i have asked too many questions in a single post

peteroznewman posted this 21 February 2020

1) i am using fixed support at one end. i am trying to apply velocity in only one direction( in this case z direction).

• Don't use fixed support.  Is the material glued to the platten or is it free to move on the platen as it deforms? Don't use velocity, use displacement.

2) i have stress-strain data obtained from compression test results that i have already done in my lab.

• Good.

3) i have used multiple deformation speed for compressing the specimen. ( values are 1.35,1.5 4.5, 13.5, 25(mm/min))

• Irrelevant. These are all equally slow from a material failure point of view.

4) i have done compression till whole material has collapsed. (i.e. till the time when the hexagonal hole( cell) present in the specimen is closed and complete crushing of the specimen takes place.

• How does the material collapse?  Ductile flow into the space, or brittle cracking?

5) the time till  which  compression is done is dependent on deformation velocity( higher the deformation velocity lesser the time taken for compression).

• You will do a displacement, not velocity. Time will not be relevant.

6) please till me about the basic process to follow to simulate this test in ANSYS. I am unable to understand your concept of plane of symmetry. HOW TO DO IT?

• I will answer that separately.

7) should i use the data of true stress- strain curve?

• Yes.

8) please also suggest the steps that i should take to get the load-displacement , stress- strain curve which should match the curve that i get from compression test. what are the required settings to be done to get these curves.

• The simulation will produce a Force-Deformation curve that you will compare with the experimental results.

i know i have asked too many questions in a single post

saurabhiitk posted this 21 February 2020

sir

1) i have attached the snapshot of the compression test of one of the specimen below.

2) it is without any support at the bottom.

3) i have also attached the snapshot of specimen when it has completely collapsed.

4) please suggest me the steps to be followed to do this analysis as soon as possible.

3)

peteroznewman posted this 21 February 2020

Do you have force-displacement data collected in a tensile test sample from a solid sample of the material in this shape?
Was an extensometer attached to the sample to measure strain in the center portion?

Is that what you mean when you say you have Stress-Strain data on the material?

saurabhiitk posted this 21 February 2020

sir

1)i have the stress- strain , true stress-true strain, load-displacement data for tensile test of ABS specimen of same shape as posted by you.

2) i do not think extensometer was attached to the specimen

3) i also have stress-strain, true stress- true strain , load-displacement data of compression test conducted on the specimen of the shape that i posted previously.

thanks for your interest shown in my doubt

peteroznewman posted this 21 February 2020

1 & 2) Was the tensile test of the ABS specimen in the dog-bone shaped test coupon done by a professional lab?  If so, they would have used an extensometer.

If you did the test yourself without using an extensometer and used the cross-head travel as a measure of the displacement in the sample, then you have compromised the quality of the data.

At what point did the sample being tested begin necking?  You can't compute True Stress and True Strain after necking begins.

3) Using high quality true-stress true-strain data, you can build a model to predict the load-displacement data of the compression test.

saurabhiitk posted this 22 February 2020

Sir

1) I actually have the data of tensile test conducted by a senior. I will once again try to confirm whether  extensometer was used or not.

2) will i have to use the data of tensile test or compression test while defining the material in the beginning of the analysis( i.e. feeding tabular data of true stress- true strain curve for multilinear kinematic hardening ( which i am using right now)).

3) please suggest me how can i build the model to get the same curve behaviour in ANSYS as i obtained during the compression test. what are the steps that i should take?

4) my task is to compare the results of simulation and experiment.

• Liked by
saurabhiitk posted this 25 February 2020

Sir

1) the extensometer was not used during tensile test of ABS specimen. i have just confirmed it.

2) should i again conduct tensile test? ( this time by using extensometer, what if extensometer is not available?)

3) are the values of true stress- true strain obtained from tensile test going to be used for this simulation?

4) how to do this simulation step by step? what are the values or settings required to do this simulation? please guide me.

peteroznewman posted this 25 February 2020

Yes, redo the tensile test and use an extensometer. This is required to do material testing. A tensile test lab must have one. If one is not available, purchase or rent one.  If that is not possible, then send your samples to a lab that can do this test for you. If that is not possible, then you will have to download ABS stress-strain data from the internet such as CampusPlastics.com

Strain in % Stress in psi

0 0

0.264 944.19738

0.526 1810.07424

0.799 2690.4549

1.056 3464.95782

1.329 4242.3615

1.589 4916.7882

1.845 5496.9402

2.117 5981.36712

2.375 6256.93932

2.641 6338.1606

Obtain a solid cube of ABS for compression testing and do that as well.

Please show the force-displacement plot for the lattice structure you are trying to simulate.

How much of that curve do you want to simulate?

saurabhiitk posted this 25 February 2020

sir

1) this is my load- displacement curve obtained from compression test at deformation velocity of 27mm/min . i want to simulate all of it ( if possible) because i will have to compare the results obtained from compression test and simulation.

2) i will not be able to do new tensile test or compression test in the lab of my institution for another two months atleast  because the slots have already been allotted to the others. it is difficult for me to wait for so long.

3) should i take data of compression test of a ABS specimen also from internet.?

4) assume that i get a new slot for compression test. what should be the size of the cube specimen and at what deformation velocity i should do the test.?

4) assume that i already have all these data ( as mentioned by you) what should i do step by step to simulate the tests in  ANSYS.?

5) Please guide me through it.

peteroznewman posted this 26 February 2020

A model that simulates the Load-Displacement curve up to 10 mm of displacement could be relatively straight forward and could be accomplished using the plasticity material model using the tensile stress-strain data.

After 10 mm of displacement is when cracking develops in the structure.  Tracking the loss of stiffness after 10 mm requires simulation of cracks in the model which is difficult.

Even more difficult to simulate is the part of the curve starting around 20 mm when the stiffness increases. This is probably due to adjacent faces of the structure making contact and providing new support.  That may be difficult to do in a Static Structural model.

• Liked by
saurabhiitk posted this 26 February 2020

Sir

1) i will be happy to know the steps to simulate it till 10mm only. please give me step by step instructions.

2) i have conducted tests on 24 samples under different strain rates. the samples are of different designs but all of  them have cellular spaces( some have circular spaces and some hexagonal spaces). that means i have 24 different load displacement diagram. please give me a general procedure to do the simulation for all these samples.

3) What is the difficulty in simulating it after 10mm?. Is it too difficult to do? what are the steps required to do it? is it possible for you to guide me through it.? It could have been better to do the simulation till 20mm for my thesis.

4) if it is too difficult to do this simulation for after 20mm. I will leave it as it is.

peteroznewman posted this 26 February 2020

A simple model is to use symmetry. Put three orthogonal planes through the center of your solid and Split the body three times. You now have 8 pieces. Keep the one piece in the positive quadrant and delete the rest. You will use three displacement conditions on those three cut faces. On the +Z face of the 1/8 model is where you need a thin block larger than the 1/8 body to press down on it. The symmetry plane on the -Z face of the 1/8 model will support that load.

Bring those two bodies into Mechanical. Symmetry BC means a Displacement of X=0 and all others Free on the face whose normal is parallel to the X axis. Make two more displacement BCs for the Y and the Z faces that were cut with planes.

Create Frictional Contact between the +Z face of the sample and the face of the block touching it.  The block face must be the Target side of the contact.

Assign the ABS material model with Multilinear Plasticity to the sample.

Create two symmetry BCs on the X and Y faces of the block. That will allow the block to move along the Z axis.

Create a Displacement BC on the top of the block with a -5 mm Z displacement, leaving all other DOF free.  When you squash a 1/2 symmetry model 5 mm, that is equivalent to squashing the full model 10 mm.

Under Mesh, set the element size so that there are a minimum of 8 elements across the wall thickness between cell cavities.

Under Analysis Settings, turn on Large Deflection, turn on Automatic Time Stepping and set the Initial and Minimum Substeps to 100.

Under the Solution Information folder, set the Newton Raphson Plots to 3 and set the Element Violations to 3.

See how far the solution gets.

saurabhiitk posted this 28 February 2020

1) Put three orthogonal planes through the center of your solid and Split the body three times. You now have 8 pieces. Keep the one piece in the positive quadrant and delete the rest. You will use three displacement conditions on those three cut faces. On the +Z face of the 1/8 model is where you need a thin block larger than the 1/8 body to press down on it. The symmetry plane on the -Z face of the 1/8 model will support that load.

HOW TO DO IT? DID NOT GET IT. can u explain it to me pictorially?

i created the part in SOLIDWORKS. can i redesign it there itself. .? if so  WHAT SHOULD BE THE FINAL DIMENSIONS OF SPECIMEN TO BE USED FOR SIMULATION.?

peteroznewman posted this 28 February 2020

• In SolidWorks, File, Save As and choose Parasolid as the file type.
• In Workbench, Drag out a Geometry component. Right Click on that and select New DesignModeler geometry.
• In DesignModeler, File, Import External Geometry File, select the Parasolid file.
• Close DesignModeler.
• In Workbench, File, Save, then File, Archive and save a .wbpz file.
• Reply and say what version of ANSYS you are using.
• After you post your reply, use the Attach button and Browse to the .wbpz file, then upload.

saurabhiitk posted this 29 February 2020

Sir

I am using ANSYS 18.0 version.

i have attached the .wbpz file below.

Attached Files

peteroznewman posted this 01 March 2020

I don't have that version. I used 19.2 to show the following.

Pick a face on each side of the model and create a plane. Here are two of the three planes.

Now Add a Symmetry object and use the 3 planes.

Now on the face whose normal is parallel to Z that is not the symmetry plane, make a sketch and draw a rectangle. Then create Surface from Sketch.

Close DesignModeler and open Mechanical  Change the Surface from Flexible to Rigid. Add a Translational Joint to ground along the Z axis on the Rigid Surface.  Add a Joint Load to Static Structural of 5 mm Displacement.

Add a Frictional Contact between the Rigid Surface and the top of the solid body.

Add a Mesh Method of Sweep to the solid. Sweep Element size = 1 mm.

Add a Mesh Sizing control to the face of the solid of Element size = 0.25 mm

saurabhiitk posted this 02 March 2020

sir

i have tried to follow the instructions that you have given me for simulation.

here are some of the doubts that i have got.

1) what should be the material and thickness of surface to be formed on one of the surface of the specimen?( MECHANICAL asks for assigning both type of material and its thickness. i have assigned it structural steel with a thickness of 5mm ( randomly) . is it correct?)

2) how to mesh the surface? is there any method for it?

3) please check the figure below to say whether symmetry plane formation and creation of surface on one of the faces is correct or not? the height of specimen has been reduced to 25mm and length of the cross section has been reduced to 11mm)

4)  I have also faced problem in setting frictional contact. but i have tried to do it. i have attached the figure below. please check it out.

5) i have applied displacement of 5mm as shown below. is it correct way?

6) my analysis settings below.

7) i have attached the force-displacement diagram below. i got it by plotting force reaction vs total deformation. the result is nowhere near the experimental data as posted to you earlier.

is the way of getting force-displacement curve i got above correct?if not how to get it?

8) i have attached the equivalent stress-strain curve below. it is a linear curve which is unexpected. i should have non linear region also. please check.

9) here is the material data that i have used. is there any mistake in it. i have used structural steel as a material for surface( as mentioned above). also i just copied the data from campusplastics website for multilinear isotropic hardening stress-strain table. is this correct?

10) i have got all this result without using any face sizing. because if i use face sizing the problem just does not get solved.

11) please see the solution information below. it is as per your instructions.

i know this is along post. i am sorry for that. but it is wise to clear as many doubts as possible in a single post.

peteroznewman posted this 02 March 2020

1) Any material, any thickness. That is irrelevant. You will assign it to be Rigid.

2) Default mesh is fine, it is not important, since it is flat and will be a Target surface.

3) Did you see three faces light up in DM after you completed the Symmetry item?

4) Good.

5) You could use this instead of the rigid surface and the contact. But it forces the whole face to remain in a plane. It is more realistic to use a Translational Joint between the Rigid Surface and Ground, then apply a Joint Load type=displacement on the Joint of 5 mm. That way, part of the face can lift off the rigid surface as it deforms.

6) Good.

7) Make the changes in #5 and #9.

8) Don't plot that, you are trying to match the force-displacement curve.

9) The material data is wrong. The first number in the stress column is the Yield Strength. Read how to create Multilinear Hardening.

10) You need at least 4 elements across the wall thickness.

11) Good.

You might need to apply some geometric imperfection to initiate failure closer to the sample data.  How many samples were tested?  Do you have an overlay of their force-deflection plots?

saurabhiitk posted this 03 March 2020

sir

i have followed the instructions given by you for material data. as given by you in #9 in your post.

i have some doubts. the young's modulus value that i have taken is 1850Mpa.

1) the plastic strain is coming to be all negative. i have used the campusplastics data points. what to do?

2) the data points that i used is below.

3) material data from campusplastics.com is given below.

4) the formula used are posted below.

5) the obtained results are posted below. the plastic strain is negative for all but one row.

what to do? please correct me if i have gone wrong somewhere.

6) i have tested 24 samples of varying designs. i have obtained force-displacement diagram for each of these samples. should i post the diagram alongwith the sample design here?

7) i also wanted to compare the stress- strain curve obtained from experiment and ANSYS simulation. what to do? please tell me.

peteroznewman posted this 5 weeks ago

1) Plastic Strain is 0 below yield strength by definition. Don't calculate it.

2) All this data is below the yield strength. You should look for data that is above yield.

3) okay

4) Correct

5) see #1.

7) What is your definition of Area you use when you divide the Force to get the stress?  Is it for the outer dimensions and includes the air in the channels?

saurabhiitk posted this 5 weeks ago

sir

1) i have corrected my material data as per your instructions.  i have used the tensile stress-strain data obtained from my lab ( without using  extensometer). i know it is a bit inaccurate as told by you earlier. i did not have any other data with me. the yield stress that i have used is 29.5MPA and young's modulus is 1043 Mpa. if u have any other data of ABS please send me. here is the image of the material data that i have used.

2) i was not able to add translational joint as instructed by you. i just do not know how to apply it. i tried my best but i was not able to do it.

3) i was able to apply face sizing this time. but element size that i have used is 1mm. and not 0.25mm as per your suggestion. i have posted the image of mesh below.

4) the force displacement curve has not changed as compared to last time. as per the experimental data obtained from compression test for 5mm displacement the force value reaches around 20KN. from simulation it is just around 4KN. that means there is some error in my formulation an ANSYS.?

5) i also have some doubts in creating symmetry plane in design modeler. i have posted the snapshots below to show face which gets highlighted after i click on symmetry  button in DESIGN MODELER.

If it is wrong. can you guide me again?

6) can you give me your email id so that i can send u the force displacement diagram of each of the samples that i have tested? it will be a bit inconvenient here to post all the diagrams with their design specimen. but if you insist i will post all the diagrams here itself. actually i have tested each design for four different deformation velocity. is it necessary to post all these? or posting Force-displacement diagram at any one strain rate will do? if you want to contact me on mail my email id is: saurabhsnh6@gmail.com

7) i think i will just use the outer area without considering the area of cells. because as per the report that i have got from compression test only outer area has been used.

8) also to plot the force-displacement diagram. i go to probe-force reaction in solutions and then plot it against total deformation. is it correct?

9) can i post the entire file of my simulation in .wbpz file for you to check my work.? although i use ANSYS 18.0. is it possible for you to check my work on ANSYS 19.2.( this is the version you have)