Zero force in all connectors' output...

[M MOTAAL]

I have a model in which i have defined fastener connector section to simulate self drilling screws in a cold formed sheet. I have chosen a connector sec. of type Cartesian and Align for the connection.The reason why I selected these types of connection; is that I needed to provide a failure criteria for the software to stop the analysis when reaching the shear capacity of the screw. And as far as I know, this criteria can be defined by defining lower and upper forces bound during defining the section within a predefined orientation in ABAQUS.
Is this a right choice(Cartesian and Align) or there is another better selection?. That was my first question and the second is about the connector output, how can I demonstrate the internal forces within the connector element? I have defined a field output in which I requested for connector elements results like CTF, CEF and CU but when I try it all the results are zeroes. So I think that I have missed something in the whole definitions procedure.
Thank you in advance.

 

[FEA way]

Did you define connector behawior too ? Take a look at the documentation for detailed description of available options. Instead of connectors you can also use regular beam elements with coupling constraints connecting them to the sheet.

You may find the article "Modeling Bolted Connections with Abaqus FEA" at Simuleon blog interesting. There are also some papers strictly about your problem. Their authors use either connectors or beams.

 

[M MOTAAL]

Hi FEA way and thank you for referring me to the article. It was actually a useful addition my knowledge. About your question if I have added behavior to the connector section or not, yes I have defined a failure criteria to the section of type "Failure" to the available CORM in the Cartesian category with bounding forces to represent shear forces of value that equals 7000 Newton (7kN) according to the manufacturer. This value was assigned in direction 2 and 3 while direction 1 is the longitudinal direction representing the axis of the screws in which I have assigned a testing value that I am still not sure about of 10,000 N (10kN)just to test the failure in tension if it works or not. I still get zeros in all types of connector results. The analysis and the job run well but the problem of maintaining the internal forces still annoying me. Did I miss something? I have followed all the documentation instructions point by point. I really need to extract these data to make sure which connector will fail first.
Thank you for your time again.

 

[M MOTAAL]

So sorry, but I have found a warning message telling the following:
"Output request s is not available for element type conn3d2"
I did not look carefully at the warning messages but I have found it out just few minutes ago.
I don't know if it is related to my issue but I have defined the field output
requests as I have mentioned before. Waht is the meaning of this message?

 

[FEA way]

Apart from Failure add also Elasticity as a behavior (in the loading direction). Connector must have a stiffness to generate forces.

Don’t worry about this message. It only tells you that stress variables from the group S are not available for connector since connectors have their own output variables (names beginning with C).

 

[M MOTAAL]

Thank you FEA way very much, but it still giving that damned zero.
but I have a one further question are these output only available in explicit solver? or it's also available in General-Static and Riks in implicit CAE?

 

[FEA way]

Make sure that your failure criterion is not making the connector fail (and thus loose stiffness completly) at the beginning of the simulation. Try solving the problem with no Failure behavior (only Elasticity).

These connector output variables are available in Static General and Static Riks too.

 

[M MOTAAL]

I appreciate your help FEA way. About your question if the failure criteria is activated at early stage of the solution and subsequently losing stiffness completely...I have to tell you that the model is thoroughly contact-free i.e has no contact or interaction and all the load has to be carried by the connector elements. The shiny side of the issue is that the model runs perfectly up to the end of loading and giving excellent fit to the verified data. but I need to enhance the model by adding the option of controlling the simulation process via a predefined failure criteria assigned to the screws especially that as I have mentioned, the load is transferred between the sheets completely through shearing forces in the connector sections. That is the reason I have to monitor the screws internal forces during different stages of loading. I also have tried different behaviors separately each at a time and combined in different arrangement but no results are yielded. All what I could make sure about now is that some components are available only as field outputs and others on the other hand are available only as history outputs. Even after I have realized this point, software still not able to catch these data even when I seek the CFAILST (Connector Failure Status ) it gives me zeros in the status output cells.
I don't know what I am missing up to the moment. Here are the steps I followed:
1. Creating a section with type of Cartesian and Align.
2. I have created in the connector section manager
four different types of behavior, they are as follows:

a)two of the four are failure behavior with bounding values of shear in direction 2,3 ranging from (-7000,7000)corresponding to (min,max). Each behavior of these two behaviors were defined at a time in the section with full release of all degrees of freedom when failure takes place as a selected option.​

b)The third behavior was the same as the previous two behaviors except for the value of range was set to be (-10000,10000)as (min, max) to represent pure tension as internal force may generate a pullout force on the screws (connectors).​

c)The last behavior was added to meet your kind advice of adding an Elasticity behavior with values in (f1,f2,f3) as210000,210000,210000) for elastic modulus of steel screws.​

3. Created attachment lines to be assigned the previously created connector section with their sets as well.
4. Assigning the sections to the attachment lines sets.
5. Requesting for all possible field and history output data for the attachment lines sets.
Do I have any missing part during these steps?

 

[FEA way]

1. How are these connectors (wire features with assigned section) connected to the metal sheet ? Through coupling ? Which type ?
2. When only Elasticity is used as a behavior are there still no forces ?
3. Can you attach your .inp file ?
4. Keep in mind that the unit of elastic stiffness defined in Elasticity behavior is F/L (e.g. N/m or N/mm) so it’s not the same as Young’s modulus.

 

[M MOTAAL]

I didn't use any type of coupling, should I? Instead I have created attachment points on the surface the created the wire frames using the projection feature in ABAQUS and selected the second surface as a target surface. Then assigned the sections to the created wires.
I am not able to send the input file currently.I think this is the point the coupling but I am not fully sure especially when I was importing the input file before so many error messages appeared pertaining to wires frames that were not created due to issues with the end points. I thought that the input file was corrupted. but now you emphasize the point of interest.then how should I define coupling? Is it like ordinary coupling in its three types kinematic, continuum,structural as usally we define set and node regions?

 

[M MOTAAL]

But if so, how did the file submit and give deformation and load-displacement curve that was really good fit to the experimental work?
I am sorry being headache to you FEA way. And really appreciate your advice.

 

[FEA way]

There are several ways to model such connection (for reference, apart from the Simuleon article, I recommend the book "FEM Idealisation of Joints" by NAFEMS if you can access it somehow). Personally, I would use coupling constraints to attach the connector to the sheet metal. Kinematic will be fine but you can use any type - they pretty much only differ in terms of how stiff they are. Try with coupling and Elasticity only and see if the forces are generated. The best way is to connect it to the small (having approximately the size of the washer) annular surface around the hole in the sheet metal.

Feel free to ask as many questions as needed to understand everything clearly - I am glad that I can help you.

 

[M MOTAAL]

Thank you for your kind reply. But if by using coupling constraint I have eliminated the job of the connector...I want to make use of this feature in ABAQUS. Especially that its much easier and accurate method(in my case at least). I also want to point out a point that I am not using holes in simulating the screws. The idea of creating a hole may be useful if I were simulating solid elements where I can make section like that was done in the Simuleon article, I think. Creating a hole may have applications also in modelling bolts with large diameter where elastic springs is an ideal solution to avoid simulation of actual bolt with solid elements and to show the damage in the metal sheet which often will be defined as 3d solid elements also.... but my case is a little bit different where there is no need for simulating the screw whole (which is of a diameter 5 mm or 0.2'') and in the same time can make use of the connector behavior provided by ABAQUS to study if this tiny-diameter screw has failed prior to reaching the maximmum load or not. This is a winning trade for me...no need for holes but in the same time controlling the analysis and knowing when to stop due to failure of the connection. So how is the coupling being defined without losing these great advantages?

 

[FEA way]

Your approach seems fine but I would try other methods (those mentioned before) to check if the reaction forces will be generated. Before doing this take a closer look at your current results. Make sure that the connector extends together with the deformation of sheet metal. If it's not generating any forces nor failing (CFAILST output variable would reveal that), it seems that it wasn't properly attached to the rest of the geometry.

 

[M MOTAAL]

It works!!
I have found out the missing part...I was defining the the interaction module via a python script in which by mistake, I defined the section of the connectors prior to defining the discrete fastener. By rearranging the code every thing works fine now except for the connector failure status it still giving zeros in the history output.
Thank you for your help FEA way. Now and after theses improvements in the situation, would you kindly, if you have idea about how to make this part work too. I also have a question about the values of Elasticity definitions for the connector sections. You have mentioned that these three values ("D11", "D22" and "D33") bear units of stiffness... is there a specific value to feed the software with it or it's dependent on the screws geometry, and if any where can I obtain such data or to be more clear I have a catalog from the manufacturing company,under which property name can I find this stiffness?.
I also want to understand the total force in connector and it's physical meaning... I know it's two components elastic and plastic but what does it refer to? Do the components mean ordinary normal and shear? or they have another meaning.
Thank you again.

 

[FEA way]

Try lowering connector failure criterion values and check CFAILST to see if it fails. When it comes to elastic stiffness specified in Elasticity behavior, it's basically spring stiffness. Just an approximation. The way of selecting appropriate value is rather empirical. Often based on the results obtained from simulations with different stiffnesses (then the one that best fits real-life behavior is chosen for the final analysis). It's probably also possible to derive it experimentally. Some values should be also available in papers where similar approach was used for bolt modeling.

Connector force is just a reaction force generated as a response to external load to which connector is subjected, due to its compliance. Total force is calculated using the following formula in Abaqus:

total force = elastic force + viscous force + uniaxial force + friction force + reaction force (caused by kinematic constraints, connector locks and stops as well as prescribed motion) - concentrated force (caused by connector loads)

Components only define direction according to specified coordinate system. For example CTF1 is a force in the X direction.