Support to fix +Uz in the same time enable free -Uz

[EngineerMickeyMouse]

How would you create support in one point with: positive +z translation fixed constrain and simultaneously (in the same point) negative -z translation free ?

Regards !

[AstroJohnPE]

Hi EMM,

These are the basic steps to do that (one-way constraint):

1. Draw a line in the direction of the constraint. The line(s) need to be on a new part number so that you can define the element type. The length of the line does not matter in most cases; choose something convenient. (Large displacement in a nonlinear analysis may be the exception.)
2. Define the element type to be gap (linear static stress) or contact or coupling (nonlinear stress).
3. Define the element definition. For linear static stress, whether the element acts in tension or compression is set in the element definition.
4. Apply a fully fixed constraint to the free end of the line.

Note that there are a number of ways to create lines. "Draw > Line" is the obvious method, but you can also copy lines, etc. If you have multliple "elements" where you want a one-way constraint, you can select the lines of the elements, duplicate them to a new part number, then copy the duplicate lines in the proper direction with the "Join" option activated. Since you only need the "joined" lines, the copy and original duplicates can be deleted.

The direction of the line ("up" or "down") usually doesn't matter. If drawn in one direction, the gap element needs to work in compression. If drawn in the opposite direction, the gap element needs to work in tension. Either option will work.

Gap elements also have the capability to include a gap before the element works in tension or compression.

Be sure to review the page "Perform Analyses with Gap Elements" in the documentation.

[EngineerMickeyMouse]

Thanks, just minute ago I figured it out, and then see perfect post from your side.

However I need more good practice regarding copy of the line. Please see picture below. Is there an option to select surface and then vertices as subentities selection and now place with one click all lines which will be later used as gap element? Surface is too complicated, there is too many nodes to copy each line by hand, also there is no pattern so any row order could be copied neither.

[EngineerMickeyMouse]

John,

I appreciate your professional responses, however the one I need now is with higher priority then previous query. 2nd question is more valuable in this case.

Kindly please advise what about many lines to be provided from vertices.

[AstroJohnPE]

Hi,

It's not clear from your image if the surface is flat or not. I'll assume that it is, in which case you want to select LINES and use the "Move or Copy" command with the "Join" option activated, as described previously. The attached image shows the process.

[EngineerMickeyMouse]

Thanks John, right that is how it works, but...

I am using batch file to solve model, since I find it much faster than using software directly.

In this case, with gap elements it is going through non linear process, so 2 questions for batch command line:

1. How we can set quantity of iterations to be performed during analysis?

2. How we can set satisfying convergence value which will finish the iterations?

Mickey

[EngineerMickeyMouse]

By iteration I mean picture below... As I assume solver is checking if gap element is closed? I am not so sure, since gap element was check on in definition for 'compression without gap' to omit gap size.

By controling value of iterations I meant iterations shown below.

John, may you put some light how to interpret process properly and in this point of view please refer to questions in post above?

[zhuangs]

Which analysis type are you using? Linear or MES?  For your model, whether is it statically stable?  "MES with Nonlinear Material Models" analysis type might be a better one.

-Shoubing

[EngineerMickeyMouse]

Static stress with linear material analysis type.

It is statically stable.

[AstroJohnPE]

Hi Mickey and everyone,

1. The number of iterations is set from the Analysis Parameters ("Setup > Model Setup > Parameters > Contact" tab).
2. There is no control for the convergence criteria, such as "within X% of the solution". Either the contact elements that are in contact remain the same for two iterations, or the solution needs to continue. (Other analysis types such as thermal can get within X% of the converged temperature, which the user can adjust to make the analysis faster at the expense of accuracy.)

I have had success changing the contact iteration method from “Mixed” to “Multiple”. This control is also on the "Setup > Model Setup > Parameters > Contact" tab. My notes also indicates that contact models will solve with the iterative solver, but it appears that the sparse solver is always chosen by default. (The sparse solver is slower than the iterative solver on large models, and 1.3E6 equations in your analysis qualifies as a large model.) My guess is that this was done because the sparse solver can handle under-constrained iterations better than the iterative solver, so make sure the model is well stabilized before changing to the iterative solver. (somewhere under the Analysis Parameters)

The page "Perform Analyses with Gap Elements" in the documentation describes the iterations that you see on the screen (and in the log file when you run the analysis through the software). Come to think of it, I do not know what "close" and "open" mean when using tension Gap elements. My guess is that  "closed" tension element is able to transmit tension, and an open tension element does not transmit tension or compression. (Naturally, a closed gap element transmits compression, and an opened gap element does not transmit compression or tension.)

I think the best thing to help with the contact iterative solution is to make a statically stable model without relying on the contact elements. That is, if you were to define the contact as "Free" instead of "Surface" (or suppress the Gap elements for a hand-built contact model), the solver should be able to find a static solution. This is normally done by applying "weak" 3D springs to each subassembly in order to create the needed stability. (I'm calling a group of bonded parts a "subassembly".) The page referenced above gives some guidelines on setting the stiffness of the springs in order to make them "weak". (I checked an old version of the documentation, so I do not know if the new documentation refers to "3D springs", or if it still refers to the outdated terminology "rigid boundary".)

[zhuangs]

Iff without those gap elements, is the model still statically stable as well?  If no, "MES with Nolinear Material Models" has to be used.  If yes, for the Static Stress analysis type, we miight reduce the stiffness of the gap elements.

-Shoubiing

[EngineerMickeyMouse]

Yes, without gap elements it is stable, solution runs correctly. I will try with smaller stiffness...

[EngineerMickeyMouse]

Choosing Multiple contact iteration and iterative AMG solver type helped with converged the model with Gap elements.

However, now again, for Gap elements I am using stiffeness to gain expected displacement of the structure. How I did noticed, this goes into vMises higher then yelding stresses, so I should use rather nonlinear analysis type than static linear.

But, here there is no Gap elements for this type of analysis. May you reconcile how to simulate these in this case?

[EngineerMickeyMouse]

John, may I ask for help?

[AstroJohnPE]

There are three options in MES to create a "one way" constraint. (One option more than in linear stress)

1. You can use the same procedure as the linear stress model with gap elements. The equivalent element type in MES is "Contact" element. It also has a few more options to define the contact element properties, but it is basically identical to the linear gap element.
2. You can model the "ground" as another part and create surface contact between the parts. You can constrain all nodes on the ground. (This same option is available in linear stress, too.)
3. If the "gound" is flat and perpendicular to the X, Y, or Z axis, you can define an impact plane.

I hesitate to mention the following, but it can have an effect in some MES analyses. MES is normally setup to perform a large displacement analysis, meaning that the direction of contact can change throughout the analysis due to the displacement of the model. So if using method 1 (contact elements to simulate "the ground"), you should make the contact elements as long as possible so that the contact force remains perpendicular to the surface. If the contact elements are short and the part moves a distance comparable to the length of the contact element, the direction of the elements and the contact force changes. This introduces side loads on the model. And if the part moves too far, its possible that the vertical component of the force in the contact element will no longer support the load at which point the part will "fall through" the support. See the attached image.