Vertical deflection of the beam - simulation

[Anonymous]

Hi

I have prepared the simplest simulation of the bodies system - beam supported on two prisms, pressed vertically - and I have some questions.

1.Everything has been correctly defined but ADF 360 wants else. What ?

The beam is properly received the all degrees of freedom (constraints), adding anything distorts the graphical result the calculation.

2.Is the result right or wrong , because he DOF view shows that the beam is potentially fixed ?

[innovatenate]

It's best to start with something you can verify the hand calculations for. Here's an example of how to do a beam analysis with hand calculations.

First, create a model with specialized face splits for constraints and structural loads.

I used one fixed constraint and one frictionless constraint to insure the correct DOF's.

Reference a standard section so that you can get the inertial section properties with ease. (I'm too lazy for hand calculations at the moment). 🙂

Referencing the below link, which is a good reference for how to do a beam analysis in Inventor Stress Analysis, the deflection equation is

http://beinginventive.typepad.com/being-inventive/2011/12/how-to-mind-your-ps-and-qs.html

Deflection =PL^3/48EI

P = 1000 lbf

L = 120 in

E = 30458000 psi (Young's Modulus from Material Properties)

I = 740 in^4

Deflection = (1000*120^3)/(48 * 30458000 * 740) = 0.00159723713 in

The results are within (.00163-0.00159723713)/.00159723713 = 0.02051221411 (2.05%) of the expected value. Anything within 10% is generally considered good.

If you enable adaptive mesh refinement, you can review if the results are converging. This can be helpful to determine whether or not the results are accurate.

You can review the model in the below public link.

http://a360.co/1WrZ2XF

I hope this will help. Please let me know if you have any other questions.

Thanks,

[Anonymous]

Hi Nathan

Thanks for your perfect response for my second question.

But what with first problem. I wanted to perform the simulation of the spring beam loosely supported on two prisms. ADF 360 wants constraints ( for green "solve" icon ) which are changing conditions of the simulation.

Regards

Ludwika

[vex]

Constraints are just the term to describe boundary conditions. IE: Fixed, Pinned, etc.

You should be able to 'pin' the line of the split faces. This should directly correspond to your original model without the need for prismatic geometry to simulate the two fulcrums. A pin constraint will allow rotation along a specified axis without translation, where as a fixed constraint will stop rotation and translation of the component.

[Anonymous]

Hi Vex

Yes, for the prism you are right , but model looks better with this two prisms 

For the "Pinned" structural constraint type this two lines which split bottom face are invisible.

After spliting this three faces may be use in "Fixed" structural constraint type with Uy axis free. The results of the simulation are correct , but the beam is still potentially fixed ( yellow light for icon ).

This sumulation is simplified : the beam is perfectly elastic and there is not the friction. I think that the friction could be simulated by the "Sliding (No Separation)" contact type - for this ,two prism models  are necessary already. The deflections of the beam ends are smaller. It can be compared with first clip.

Regards

Ludwika

[innovatenate]

To get to the central question, the yellow solve light is only a warning that some of your bodies may not be fully constrained. This may be true as I could not see the contacts in your video. I noted that you added a fixed or frictionless constraint to the bottom faces of the wedges. However, the relationship between the beam and wedges is unknown to me without knowing how the contacts are defined.

Contacts are user defined relationships between different bodies/components. They control the way that bodies interact with one another. The DOF View command (under View menu in SIM), can help you to determine how the current constraints and contacts interact with one another. You can quickly get a sense of which bodies are "locked down."

This can be really valuable when doing a more complex simulation on a design containing many bodies/components with varying types of contacts.  The DOF view can allow you to quickly figure out which groups of bodies are “stuck” together or are free to move. Below are descriptions of different types of contacts and how they can impact the DOF's of adjacent bodies/components.

Bonded contact: Think bodies/components being "welded together." This is a linear contact type where deformation results will be equal for adjacent nodes on either body. The result is that multiple bodies or components will be treated like a single body. This contact does not allow penetration or sliding to occur. The DOF’s for one body will be the same for another body that shares a bonded contact.

Separation - Sliding: This is a frictionless contact where separation in the normal directions and sliding in the tangential direction is freely allowed. Note there are no “frictional” forces associated with this contact type. The contact will allow for DOF’s between two bodies to be separate. Further constraints may be required to modify the DOF’s for each body.

Sliding/no separation: A frictionless contact where no separation is allowed between the parts but they can slide tangentially to each other, freely. In this case each body/component may be treated with different DOF’s since each body can slide without causing a reaction in the other body in the contact.

 
Separation/no sliding: This is a frictionless constraint. It's similar to a separation contact because it does allow gaps or separations to occur, but no penetration. If the faces are in contact, then no sliding in a tangential directions is allow to occur. In this case each body/component may be treated with different DOF’s since each body can separate in a normal direction without causing a reaction in the other body in the contact.

I hope that helps with the understanding of the DOF’s and what is happening between the beams and the fulcrums.

[Anonymous]

Nathan

Many thanks for your comprehensive and clear explanations.

But let me he one more question.

If , I quote, "Sliding/no separation: A frictionless contact where no separation is allowed between the parts but they can slide tangentially to each other, freely. In this case each body/component may be treated with different DOF’s since each body can slide without causing a reaction in the other body in the contact."

Why is  the deflection of the ends of the beam smaller when the Sliding(No Separation) contact type is defined, then in the case ,when any contact is defined ? Watching this two clips

https://www.youtube.com/watch?v=mRJw5MHQzeM

https://www.youtube.com/watch?v=E4P0n44H7RM

you can see it  very clearly. This clips are made 1080HD resolution.

Of course the presence of the beam has no influence for the prisms ( shape ,deflection, etc.) ,but the deflection of the beam is other.

I do not want to be too scrupulous but I can see this differences clearly.

Is the simulation with contacts defined , more realistic?

Thanks for your patience.

[innovatenate · Accepted solution]

Can you describe better what the end conditions of the beam are or what the goal of the simulation is? Is this supposed to be a simulation of a simply supported beam (vs. cantilevered, etc..)? The end conditions make a big difference in how I would approach the simulation.

I'm assuming one end is "pinned" and the other is going to act like a roller and allow for free translation in the Ux direction for a "simply supported" beam. Is that correct?

An odd constraint in both of the simulations has been apply to the bottom face of the beam. You have left Uy free, but fixed displacement in the Ux direction.

 As the board bends, the elements in tension will elongate while the elements in compression will shorten. 

The nodes on the beam should be free to displace in the Ux direction as the beam deforms (or at least I think so - it depends on the boundary conditions). You'll note in the above results that the right prism was allowed to move in the Ux direction and the beam elongated, displacing the support. This existing constraint could impact the results of the simulation. As a beam bends the nodes will need to be free to move in the Ux and Uy direction. To help with the DOF issue, one end maybe pinned or fixed.

This may also explain the differences in the deformation when you change the contact types. In one scenario you've defined the contacts to be sliding + separation and in the other you've selected sliding (no separation). In both, I'm assuming you've fixed both of the prismatic supports in all directions. Depending on the nodes that have utilized in the contact, the restriction of the no-separation contact may impact the displacement in the Uy direction. This coupled with the elongation issue I mentioned above may be working together to change the deformation results. Some things you can try to combat this:

• Split the face of the beam where the supports meet. This will force the mesher to create nodes that line up with line contact of the supports. 
• Decrease the size of the mesh to create more nodes to be shared in the contact
• Change the value of the contact tolerance in the Simulation Settings

I'll note that the deformation results, the values themselves don't appear to be significantly different, but I do think that the above information may help to explain the differences you are seeing. Let me know if you have any questions.

[Anonymous]

Nathan

Your last post explain me everything. My last questions was wrong. I forgot that in last study the prisms were hidden.

Thanks for your patience and for taking me so long. I am grateful to you for help me in understanding of issues constraints and contacts. This three posts from you ,will be base for my furthery study. Thanks.