Hello, how can I help?

OWW! That's great Mr. Ali Kara. Now I am doing (practicing) the simulation of "Split-Hopkinson Pressure Bar"  by ANSYS LS-DYNA. I need multiple assistance regarding it. I hope you will not feel bad, to keep conversation about it.

For the 'Transmitted Bar' - What type of boundary conditions I have to choose?

It is OK. For the transmitter bar or the other bars, you don`t need to define boundary conditions if your model is a full model (if it is quarter, you have to define symmetry BCs). In LS-DYNA there is no gravitational forces, unless you add it. Then no other force applied in the simulation except for hit of striker bar (or incident wave applied to the incident bar face). Therefore, nothing like "bearings" in real experiment is needed in the simulations (actually even in real experiment bearings are smooth and generally lubricated to have a good sliding and low friction).

My model is a full scale model, so as per your suggestion, I don't need to add any boundary conditions there. May I need to define any kind of 'Spring' or anything behind of Transmitted Bar?

Moreover, adding gravitational forces is necessary - what's your opinion? Is it possible to check the velocity of the striker bar, just before hit the incident bar (Actually I want to check that, velocity of striker bar remains same or not from starting to just before hitting) ?

Mr. Ali Kara, for your kind information - if I want to calculate the response at the end of transmitted bar, may I need to add some soft material (like spring) by providing some stiffness at the end of the transmitted bar? What's your thinking?

Your help is highly acknowledged, brother.   

Hi, actually you dont need gravitational forces. Align axis of bars in the z direction and dont give any bcs. In the simulation you are gonna have transmitted stress at the middle of your bar to compare it with experiment. I dont understand why you think you need spring attached to transmitting bar. Even it is so in the experiment we only care about one incident, one transmitted and one reflected wave (except for multiple reloading experiments) when your aim is to validate your material. I mean we are not interested in the wave travels through the transmitter bar and reflecting back from its free end.

Laser sensors can be used in SHPB setups to find "average" velocity of the striker. For instance if average was measured as 25 but real instant velocity was 23 at contact it is not going to affect your results a lot.

Sincerely. 

Hi, ton of thanks again for your response. Ok, now I got your point. I know and saw that, during experiment laser was used to calculate the velocity. But I am talking about the checking velocity at software model. I need to check the initial velocity (it is provided by me) and the hitting velocity in model, they are same or not. How to do it in LS-Prepost (Because, I use LS-Prepost, for post processing)?

Thanks !!! 

In SHPB simulation you give it as initial velocity with *INITIAL_VELOCITY_GENERATION card (or another as you wish) and you put striker bar very near to incident bar striking face (for instance if an incident bar is 2000 mm long and striker bar 350 mm long their distance between contacting faces can be 0.00000001 mm by using LSPRE). And the velocity you define can be guaranteed that way. 

Besides if you want to check the velocity that you provide after simulation you can simply go to page 1, history, check nodal velocity along the direction of bar's axis.

You are welcome.

I understand now. If I need any more further help, I will let you know. Hope so, you will not feel hesitate to teach me :)

For Split-Hopkinson Pressure Bar test simulation by ANSYS Workbench, what type of 'Contact' I have to define?

For Split-Hopkinson Pressure Bar test simulation by ANSYS Workbench, what type of 'Contact' I have to define between "Striker Bar" to "Incident Bar", "Incident Bar" to Specimen and Specimen to "Transmitted Bar"? 

Can you please give me the "Contact" modeling idea during "Modeling" of this. 

Hello Imrose, I am not familiar with ANSYS Workbench actually. I am not sure what type of contact is included in it. Sincerely.

it's Ok!

But what about the LS-DYNA? What type of contact I can define between those?

Hello Imrose, there is a good documentation, maybe you already seen, about contact definitions in LS-DYNA. Maybe you can refer to the following for general sense of contact modelling.

http://www.dynasupport.com/tutorial/contact-modeling-in-ls-dyna

http://www.dynalook.com/fea-newsletters/fea-newsletters-2001/fea-newsletter-december-2001.pdf

But to model SHPB test, between striker and incident bar automatic surface to surface contact is OK. Between specimen - bars interfaces you may simply use automatic surface to surface contacts (may be nodes to nodes or segment based all works OK and must be tried if there is a problem). If there is erosion (damage) in your specimen (actually of course there must not be erosion in bars those are elastically modeled) you have to use eroding surface to surface contact to account for eroding pieces possibly contacting after fracture occurs.

If your specimen material is a challenging one (it may be soft like foam) you can use SOFT options of contacts. If for example your material is a harder material than your bar material (ie stiffness is higher than the bar, it is not possible in real experiment, but we can use some indent preventer disks but you dont have to model them in the simulations), you can simply scale down the stiffness of specimen by SFS.

Generally specimens treated as slave surfaces and bars treated as master surfaces. You can look up for friction coefficients through the internet between surfaces or you can use trial and error method and if it is not changing your results a lot you can select a generic friction coefficient.

Even all pieces can be included in one Automatic/Eroding_Single_Surface card and Force_Transducer_Penalty card can be used to determine contact forces.

For contact forces you have to include a DATABASE_ASCII_OPTION RCFORC must be checked and must be assigned with a DT which is generally (or can be) smaller than the DT of the d3plot.

This is all I can imagine right now. You can ask if I forget to mention about something. Sincerely.

Hello Mr. Ali Kara and Mr. Imrose Bin Muhit

I am also trying to simulate a Split Hopkinson Pressure Bar test on a Glass sample using LS-Dyna. I am using MAT3 for bars and Mat123 with failure strain value for glass sample. I would really appreciate if you could tell me about the Eroding Single surface contact(currently I am using Automatic Surface to Surface contact) and also how can I validate my simulation(what results i should compare with the experiment). Mr. Ali Kara, you have mentioned about comparing transmitted stress in the bar with experiment. Can you elaborate more about this?

Can you please help me out with these doubts?

Thank you in advance.

Regards