Ok I have a few remarks if I may

First, 45,000+ elements is way too much for something so simple. Since your geometry is basically a 3 meters long beam, why don't you try with a few dozens to a hundred elements and see what the results look like, then maybe add more?

Second, if you use a "fixed" time increment of 10^-15 s for a 1 second simulation, you're going to get 10^15 increments... The automatic increment option is far better in my opinion, I suggest putting initial and maximum increment at 0.01s if you really need to describe what happens frame by frame, but 10^-15s is far too little, especially since you put something like 100,000 maximum number of increments.

Third, the boundary condition for the lower face of the concrete was not well specified : like Mohammad said, it needs o be defined in the initial step, otherwise when step 1 starts everything happens at the same time and so the model is not well constrained at first. Besides, if you fix U2 to 0 but not UR1 or UR3, you allow rotations to happen on this face, and I'm not certain that's either realistic or very good for the calculation. I suggest you first try using a YSYMM condition and then eventually refine it to be more representative of what happens in reality. At least I've tried this with your model and I don't have the warning messages about being zero force in the whole model.

The warning messages I do get however state that some adjusted nodes with small adjustments were not printed, also that there is a numerical singularity on degree of freedom #1 (so X translation) of a certain node (concrete 99).

Finally, you compress your concrete beam of 100mm in 1 second. Given you beam is 3m long, that 3% strain in 1s so 0.03s-1 strain rate. I don't know if that is representative of what you want to simulate, but that's already high strain rate. Look into it to make sure you're not deforming your beam faster than in reality.

I don't really have much more time to look into it, but follow my advice and you should have less trouble.

Good luck

These are usually not errors but warning messages. It just means that the different regions of your geometry are not in physical contact, and that no effort is applied anywhere.

Without knowing what you are trying to simulate, I cannot tell what the problem is, given there is one. If the calculation stopped and these are indeed error messages, I assume you did a purely mechanical simulation, but apart from that, I don't know what is supposed to happen in your model.

With more details I might be able to help.

Please check your contact ..... abaqus has a general contact and you can do exception ..... anyway if you are not able to define contact ....... Make a tie constrain

be care to define contact and apply the load before meshing

may since I don't know exactly your geometry ..... but just trying to provide general notes may be useful

best of luck

Thank you very much for your replies,

Actually I am very new in Abaqus and thats why I make obvious mistakes.

I have attached the geometry of my model. There is a wall made from PVC filled with concrete. There are also linking webs from PVC in the middle of wall. I applied embedded constraint region between concrete and linking PVC webs and also surface to surface contact between concrete and outer shell of PVC. 

I want to use displacement control instead of the load control, so I applied 100 mm displacement on the top surface of concrete.

After submitting the job, that warnings appear.

I would be grateful If you could give me your ideas.

regards,

Mahya

please check the 2 outer webs and the mid one, probably that's not connected, try to use tie constrain between areas, in case that's a link, connect lines together

regarding the load, check the interaction between loading plate and the concrete wall, probably that you need to connect them again using tie constrain

when you are defining the interaction, be care about the color, for the web it has to be line by line i think since i noticed that u did that as a shell elment

Ok first off, could you display the assembly and selecting the "Parts" or "Parts instances" option in the color code menu? That way we can see each part better. And I don't see where the concrete is in this image, so if could add some legends that would be even clearer.

Second, it looks like the parts displayed here are meshed with shell elements, are they? If yes, how did you affect the thickness to your different parts? (more clearly, is the surface you drew considered to be middle, bottom or top section?)

Third, in what direction do you specify the displacement boundary condition? Y axis? If so, are you pressing or pulling the concrete?

Finally, if the concrete fills the PVC wall and the PVC is tied to the concrete ("glued" in a sense), why would you use a surface-to-surface contact? If you pull it but there is no tie between the concrete and the PVC, the concrete will just stretch and the PVC will stay in place, which would explain why contact is lost. As for the the webs, I guess they should be tied to the walls and embedded in the concrete.

As you see the assembly consists of just 2 parts, the PVC wall and concrete. I have merged the outer and inner shells because the wall with all components is prefabricated in this shape at factory.

Also all PVC parts have the same thickness.

I applied the load in Y axis direction as it press the concrete.

I embedded the linking webs in concrete and also defined the surface-to-surface contact between concrete and outer parts of wall as I think contact will happen in reality if I’m true, you can see the attached images.

As you mentioned, I defined tie between concrete and outer shells instead of surface-to-surface contact, but this time this warnings appear:

1) For *tie pair (assembly__pickedsurf59-assembly__pickedsurf58), adjusted nodes with very small adjustments were not printed. Specify *preprint,model=yes for complete printout.

2) There is zero FORCE everywhere in the model based on the default criterion. please check the value of the average FORCE during the current iteration to verify that the FORCE is small enough to be treated as zero. if not, please use the solution controls to reset the criterion for zero FORCE.

may you can attach the model to see loads, geometry, and boundary

Dear Mohammad,

I have attached the inp format as your Abaqus version my be different with mine

cheers

sorry i couldn't open this file

I'm using 6.13 ,,, may you can send me the abaqus file

You have to import the inp file .I cant upload the cae format here

I tried to fix it ....... define the boundary conditions to start from initial not from step 1 because boundary has to start from initial

2nd thing is the constraint ...... I think may you need to model it not like embedded element

Ok I have a few remarks if I may

First, 45,000+ elements is way too much for something so simple. Since your geometry is basically a 3 meters long beam, why don't you try with a few dozens to a hundred elements and see what the results look like, then maybe add more?

Second, if you use a "fixed" time increment of 10^-15 s for a 1 second simulation, you're going to get 10^15 increments... The automatic increment option is far better in my opinion, I suggest putting initial and maximum increment at 0.01s if you really need to describe what happens frame by frame, but 10^-15s is far too little, especially since you put something like 100,000 maximum number of increments.

Third, the boundary condition for the lower face of the concrete was not well specified : like Mohammad said, it needs o be defined in the initial step, otherwise when step 1 starts everything happens at the same time and so the model is not well constrained at first. Besides, if you fix U2 to 0 but not UR1 or UR3, you allow rotations to happen on this face, and I'm not certain that's either realistic or very good for the calculation. I suggest you first try using a YSYMM condition and then eventually refine it to be more representative of what happens in reality. At least I've tried this with your model and I don't have the warning messages about being zero force in the whole model.

The warning messages I do get however state that some adjusted nodes with small adjustments were not printed, also that there is a numerical singularity on degree of freedom #1 (so X translation) of a certain node (concrete 99).

Finally, you compress your concrete beam of 100mm in 1 second. Given you beam is 3m long, that 3% strain in 1s so 0.03s-1 strain rate. I don't know if that is representative of what you want to simulate, but that's already high strain rate. Look into it to make sure you're not deforming your beam faster than in reality.

I don't really have much more time to look into it, but follow my advice and you should have less trouble.

Good luck

Dear Etienne,

Thank you very much for your advice. I will follow them and hope to get good results.

cheers,

Hi

Did you could solve your problem with unconnected regions?

You have to be careful about adding your instance parts to your assembly. It is like Copy/Paste at paint. If you add a part for more than one time, you will have one part twice. That's the reason you have unconnected part when you run your model. In fact the parts that you added twice or more will be unconnected.

hi all,

Is it the same case if we have this kind of warning?

"There is zero VOL. FLUX everywhere in the model based on the default criterion. please check the value of the average VOL. FLUX during the current iteration to verify that the VOL. FLUX is small enough to be treated as zero. if not, please use the solution controls to reset the criterion for zero VOL. FLUX".

Best regards,

Abdo

Dear Etienne, 

I m working on precast concrete pavements connected with dowel bars.

I have the same problem of unconnected regions in the  model, what is this YSYMM condition? If u can tell me more about this condition it may help me solve my problem.

Thank You

@Mahya Askarian

Are you able to detect directly without checking which part or region is not connected please help me also regarding this warning because I have very less time.

Waiting for your reply

Mohammad Samaaneh

HELLO

I have the same warning of unconnected regions in the  model

could you help me resolve this warning,plz?

thank in advance

Ravi Suthar

HELLO

I have the same warning of unconnected regions in the  model

could you help me resolve this warning,plz?

thank in advance

Although it is too late to comment on the post but those arriving after me can take benifit from it. If there is interaction involded on those surfaces, which are sharing coordinates commen to the surface which is tied (Tied constrained) to another surface, this error occurs. To be more precisely, look at the picture i attached below, If you look at the bottom of the wall. There is a commen interface on the top of the steel section and the beds of the lower bricks. Also at the same time the lower brick wall are sharing the header faces to each other. Now if you apply tie constrain and interaction to the steel and beds or the bricks and the header faces respectively, it will be sharing some commen nodes of the perpendicular surfaces, which will give warning of conconnected regions in your model. Similar is the case with 2D problems, if the nodes are not adjusted and the surfaces are not pre defined for proper directions (By proper direction, i mean normal vector of the surface for interaction). Most often, this error arise due to the contact pairs. To avoid this error, make sure the nodes are adjusted in keyword editor or input file. Those who are suggesting that, the instances are copied twice are completly wrong. ABAQUS cannot start simulations if two instances are copied and pasted inside each other.