contact

[mambo5]

hi,
any idea what went wrong with my model? i simply put 2 plain concrete block (150 x 300mm) together, and put spring between them (as contact), my main porpose is to make sure that the 2 blocks will act as one single block (150 x 600mm), but by checking the deflection (after the matching)compare with simple hand calculation, it doesn't seem what i have done to the contact part is right.
please advise.

 

[corus]

I'm not sure how the job was able to run as you don't have enough restraints to the model. Check the msg file and you'll see warnings about negative eigenvalues.

I'm not sure exactly what you're trying to do as you define contact and yet have springs between the two bodies. I don't see the need for the predefined temperature field of a constant 20C either, but neverthelesss.

Looking at the displaced shape, the top body has moved down a distance, probably an amount given by the spring stiffnesss. If you want the two to move together then you'd need a bigger spring stiffness or just do away with the springs altogether and move the two bodies together in the assembly module and have contact.

Is there a need for finite sliding in contact as the two won't slide across each other?

corus

 

[mambo5]

i removed all the springs, and apply 'Tie constraint' between both blocks. they are fully tie together and acting as a 'single body' now, that's what i want to make sure about the 'contact' function in Abaqus, cause there are so many of them, i not really sure, which to use and what i will get by using them...

 

[corus]

In this case you have the corners simply supported, with a simple clamping pressure. You may get some sliding but you don't need finite sliding for this type of problem. Use the normal and tangential behaviour in the properties to define friction.

corus

 

[mambo5]

thanks corus,

what if i have a composite structure (concrete slab on top and I-section at the bottom, shear stud in between the slab and beam to connect both components).
I will apply tie constraint between the slab and beam surfaces, so that the 2 components will act as a single composite structure (assumed full interaction between both component, where slip=0 everywhere), correct me if i am wrong.
If i would like to consider the shear force in the stud connectors, i have to apply *spring2 or *springA between these 2 components, and set the DOF along the direction of the beam.
please advice.

 

[corus]

Slip may be zero everywhere but if you think the two may bodies may seperate under say a bending load then use contact between the two surfaces rather than tie them together. The less contact between the two via friction will mean additional load into the studs. I'd do the same as you and use a beam element embedded into the two bodies to represent the stud.

corus

 

[mambo5]

thanks corus,

if i use beam element as you said, what length should i specify for the beam element between the 2 nodes (slave and master)?
possible to attach the *.inp of the model that u mentioned? which use beam elements to represent the studs.

 

[corus]

The length of the stud will affect the axial stiffness and hence any effect on separation of the two parts. Instead of leaving a gap as you did originally, which surely can't represent the real world, why not have the two bodies in contact initially and have the beam elements the same length,area and MOI as the real studs? The beam/stud ends will then be tied to two nodes either inside or on the outer surface of the two parts.

corus

 

[mambo5]

Corus,

I trying to use beam elements as you suggested, I tied the beam elements on the top flange surface, but how could I tie the other end into the concrete slab? as Abaqus only allow me to select nodes on the surface of the component, not inside the component.
beside, do i need to define the 'surface to surface contact', for both the slave and master surface of the section (i.e master = top flange of I-section, slave = concrete bottom surface). please advice.

 

[corus]

You can simply partition the part so you have internal points at any position. Just use intersecting planes for example.
As you say, define the master and slave surfaces as the top of the flange/bottom of the concrete. For contact the master surface should be the harder of the two materials, which in this case will be the steel.

corus

 

[mambo5]

THANKS CORUS,

have you done any model for concrete material has run sucessfully in Abaqus? as i defined my concrete material properties by using *concrete keyword (case 1), i need to define the *tension stiffening as well, i used concrete softhening stress-strain curve, but Abaqus couldn't finished the analysis. So i use *elastic, *plastic keyword (case 2) to define the concrete material (i ignored the softhening part, let the plastic stress remain constant after reaching the concrete maximum stress) as what i have done to define the steel properties, Abaqus run longer than before. the thing is i could only define the concrete compressive part in case 2, but not the tension part. do you think this is the 'right' way for concrete material analysis? please advise.

 

[corus]

I've modelled both refractory brick and concrete materials and have found that the easiest way to model the materials was by simple elastic/plastic behaviour. This approach has been verified by measurements so there is a lot of confidence in the results produced, but for this particular application of course. In the cases I look at though the materials are always in compression, or at least should be. Generally I conclude that, by visual inspection, if the material goes into tension in any way then I assume that the material has failed as it basically has negligible strength in tension. The problem with thse models is the limited temperature dependent stress-strain properties available, and those that are are always from compressive tests. I tried the *concrete option once and couldn't get it to work for one case I had so I think I used cast iron type behaviour to describe different yield properties in tension and compression.

corus

 

[mambo5]

just want to double check, I am using shell element for both the concrete slab and I-section, initially i will have a 25mm gap in between both parts ( measured from bottom of slab to top flange), i applied *tie between the 2 parts in order to tie them together (as a fully interaction composite section), woundering what should I put with the 'Adjust=YES or NO' in the *TIE keyword? if i would like the gap to maintain thru out the analysis.

 

[corus]

There's an 'exclude shell thickness option' box in the contact manager in the interactio module. Leave this blank. I'd include Adjust=yes to prevent initial overclosure in case your geometry is a little out. Normally this will adjust the nodal positions so that nodes will be on the same surface but with the exclude shell thickness option unchecked then the thickness should be accounted for. You can check in Viewer when you run the job to see if the nodes have been moved more than you expect as this can give unexpected mesh errors. Use a data check analysis to do this rather than run the whole thing fully.

corus

 

[mambo5]

THANKS CORUS,

as the earlier reply (27 Feb), you mention that 'you used cast iron type behaviour to describe different yield properties in tension and compression', what do u mean by 'iron case'?
beside, u ignored tension in concrete strength in tension, was that mean u didn't apply any tension stress- strain curve in your model? and you were also using the *elastic & *plastic keywords to define the concrete properties?

 

[corus]

With cast iron I think you can define different behaviour in tension and compression, so you can apply a low yield in tension but normal 'yield' in compression. For concrete type materials you only get compressive stress-strains though so anything you apply in tension is just fictitious, as far as I'm aware. It has been practice in the cases I consider to just use *elastic and *plastic but these cases involve transient temperature dependent behaviour with contact and the whole non-linearity of the problems tends to rule out further failure criteria so that at least some meaningful results are obtained in a reasonable amount of time. If your case is simpler then I'd consider *concrete and follow the notes in the documentation. The problem, of course, is obtaining the material data for input.

corus

 

[mambo5]

I am using shell elements in my model, 'cast iron' not allow to be used for plane stress model.
by the way, in the *elastic, there are options 'No compression' and 'No tension', if I click on the 'no tension' button, is that mean Abaqus will not consider the tension stress- strain curve? if i use the *elastic and *plastic to define my concrete properties, than i will only have the concrete stress-strain curve.
please advice.

 

[corus]

If you're using shell elements then there is no plane stress option. Plane stress is for 2D solid elements where the stress out of plane can be considered to be zero, such as for thin 2D plates where the loading is in-plane.

In any case try the 'no tension' option, which presumably does as it says, and doesn't consider the material in tension. Your stress-strain data will then apply only in compression. The best thing you can do is to run the analysis and see if the results you get make sense and the material behaves as you expect it to.

corus