Simulation of Thermal Expansion. [Please help...I am so frustrated]

[ptc-5675684]

Hi everyone,

I am trying to simulate the thermal expansion of a cubic model under Global temperature load.

My question is how to constraint the model so that expansion can be seen on EVERY surfaces? For some reasons Wildfire 4.0 requires not a point, not an edge but at least one surface to be fixed in order to run the analysis.

I tried placing another model underneath and defined the interface between two models as "contact" with infinite friction enabled. However the result was totally incorrect even though expansion did appear on all surfaces.

Any advices would be greatly appreciated!!

Lawrence

[sdensberger]

My question is how to constraint the model so that expansion can be seen on EVERY surfaces?

Thermal expansion is relative; there will always be a point that has zero expansion. Are you trying to get your cube to expand relative to the center? If so, then the easiest solution is to use symmetry. Model 1/8th of the cube and constraint each of the 3 cut surfaces such that they can't move in the normal direction defined by the surface.

For some reasons Wildfire 4.0 requires not a point, not an edge but at least one surface to be fixed in order to run the analysis.

In any analysis (expect for a modal analysis with rigid body search on), you need to have your model constrained in all six DOFs to ensure that a unique solution exists. The nodes of a solid element only have three DOFs, so three non-collinear points are needed to kinematically constraint the system. You can either do this by fixing a surface in all three translational DOFs, or by picking three non-collinear points and constraining them such that they remove all six DOF when combined (this is sometimes known as a 3-2-1 constraint).

I tried placing another model underneath and defined the interface between two models as "contact" with infinite friction enabled. However the result was totally incorrect even though expansion did appear on all surfaces.

How was the result, "totally incorrect?" Did the bottom surface not expand with the side surfaces? You defined an infinite friction contact between two surfaces, so would you expect any relative planer motion of the surfaces to happen?

[ptc-5675684]

Hi Shaun, thanks so much for your prompt reply!

Thermal expansion is relative; there will always be a point that has zero expansion. Are you trying to get your cube to expand relative to the center? If so, then the easiest solution is to use symmetry. Model 1/8th of the cube and constraint each of the 3 cut surfaces such that they can't move in the normal direction defined by the surface.

Sorry my question was quite misleading. Please allow me to rephrase. I have attached a picture for better explanation.

Indeed, waht I want to achieve is the stress distribution of the Shell under thermal load as you can see in Fig.3. That's why I think I should not constraint each of the 3 cut surfaces, otherwise the stress distribution will be inaccurate.

However, having the bottom surface fixed, the entire model expands in an irrealistic way because the bottom side should also has expansion. In reality, the object is placed on a moving tray and passes through an oven at 260 degree, without being clamped or contrainted at all.

In any analysis (expect for a modal analysis with rigid body search on), you need to have your model constrained in all six DOFs to ensure that a unique solution exists. The nodes of a solid element only have three DOFs, so three non-collinear points are needed to kinematically constraint the system. You can either do this by fixing a surface in all three translational DOFs, or by picking three non-collinear points and constraining them such that they remove all six DOF when combined (this is sometimes known as a 3-2-1 constraint).

Thanks again for the amazing expalantion, I now understand why do I need a fixed surface. But by constraining three non-collinear points, stress tends to concentrate toward these points.

How was the result, "totally incorrect?" Did the bottom surface not expand with the side surfaces? You defined an infinite friction contact between two surfaces, so would you expect any relative planer motion of the surfaces to happen?

I should not have used the word "incorrect" because the analysis process itself was right.
What I was trying to say was by enabling infinite friction, the expansion and the stress distribution became so weird that I was not able to correlate the result with anything.

[TomD.inPDX]

What if you fix a very narrow strip or a dot, maybe on the side?

[ptc-5675684]

Hi Antonius,

Thanks for advice.

However it will result in high stress concentration around the corners or the edges.

Quoted directly from Wildfire4.0:

"The highlighted point constraints can cause singular stress concentrations."

Source: Solver

Lawrence

[sdensberger]

Indeed, waht I want to achieve is the stress distribution of the Shell under thermal load as you can see in Fig.3. That's why I think I should not constraint each of the 3 cut surfaces,otherwise the stress distribution will be inaccurate.

Why do you think the stress distribution will be inaccurate? Is your part geometry non-symmetric? Do you have non-symmetric loads?

In reality, the object is placed on a moving tray and passes through an oven at 260 degree, without being clamped or contrainted at all.

Are you using the thermal load on the structural side of Mechanica? This applies a global temperature change across all nodes. This means you won't capture any transient effects or stresses due to a thermal gradient; all you will capture are stresses due to different coefficients of thermal expansion or due to your constraints preventing some thermal expansion.

If all you're after are the stresses at a uniform steady-state temperature, then I see no reason why you can use symmetry (provided the above points are true). The only non-symmetric property I can think of (based off of the image you posted) is gravity (depending on which 1/8th of the model that you use), but you can easily capture that with an applied force.

Thanks again for the amazing expalantion, I now understand why do I need a fixed surface. But by constraining three non-collinear points, stress tends to concentrate toward these points.

Not necessarily. A stress singularity will only occur if your constraint results in some mechanical strain (either from the prevention of some thermal strains or some applied forces).

[ptc-5675684]

....all you will capture are stresses due to different coefficients of thermal expansion....

This is exactly the objective of the simulation! Cracks were observed near the upper corners of copper during experiments and they are believed to be casued by the mismatch between the CTEs.

I am currently reconstructing the model wihtout the use of Shell.

[TomD.inPDX]

Cadet home heaters made a huge mistake in casting heating tubes inside aluminum fins at one time. They all failed after a time. They replaced all of mine free of charge. I can certainly see your application. However, what if you extend and fix the copper parts and let the surrounding material be free.

[sdensberger]

How are you bonding the two dissimilar materials together? One thing to keep in mind is that (in FEA) the stresses at the interface between two different materials are singular if there is a difference in properties (like Young's Modulus and Poisson's Ratio). If the components are not bonded together (for example, a interference fit), then doing a non-linear analysis with contact will resolve this issue.

If you don't want to do a symmetric model, then the setup shown by Steven Dunker will work for you. The displacements will be relative to the zero displacement point, but fortunately this doesn't impact the stresses (assuming the system freely expands).

[ptc-5675684]

They are bonded by the default "bonded" interface since in reality, the components are sticked together with the epoxy resin acts as an adhesive "glue".

If I understand Steven correctly, what he demonstrates is the procedure of assigning symmetry constraints, right?

Apart from 1/8th, I also created a 1/4th model and assigned symmetry constraints to the two cut surfaces. Analysis was then performed and everything went well. The result was even quite promising! But when I tried to export an image, Pro/E suddenly crashed and closed on its own. After restarted the program and ran the analysis again without changing notihng, I could no longer achieve the same result but instead getting error message about insufficient constraint.

It is weird. There was a moment I thought I finally made it.

Anyway, I was also suggested to use the function called "Inertia relief" by a PTC technician, in order to simulate a "floating" environment. The result seems acceptable but not sure it is realistic enough because it is still difficult to correlate to the result of experiment.

[sdensberger · Accepted solution]

They are bonded by the default "bonded" interface since in reality, the components are sticked together with the epoxy resin acts as an adhesive "glue".

I assume in the failure point in the physical system was the epoxy? How thick is the epoxy layer?

If I understand Steven correctly, what he demonstrates is the procedure of assigning symmetry constraints, right?

Yup, Steve shows how to apply triple symmetry (leaving you with 1/8th of the geometry) using the "Mirror Symmetry" constraint. You could also use the standard displacement constraint and release the proper DOFs.

Apart from 1/8th, I also created a 1/4th model and assigned symmetry constraints to the two cut surfaces. Analysis was then performed and everything went well. The result was even quite promising! But when I tried to export an image, Pro/E suddenly crashed and closed on its own. After restarted the program and ran the analysis again without changing notihng, I could no longer achieve the same result but instead getting error message about insufficient constraint

For your 1/4th model, what was the third constraint that you applied?

It is weird. There was a moment I thought I finally made it.

Can you post some pictures of your model setup (or the model itself)?

Anyway, I was also suggested to use the function called "Inertia relief" by a PTC technician, in order to simulate a "floating" environment. The result seems acceptable but not sure it is realistic enough because it is still difficult to correlate to the result of experiment.

You could use inertial relief and still get good stresses, but your displacement values will be mostly meaningless. For inertial relief, the software selects 3 points on your model and applies "soft springs" (spring elements with low stiffness) to anchor the model. This process is very similar to the 3-2-1 constraint method both Jonathan and myself described, but uses grounded springs instead of nodal constraints. However, with a 3-2-1 constraint we know that all the displacements are relative to a given node on the model, but with inertial relief the model could go through some displacement large enough to "wash out" the thermal expansion displacements. For your model (just thermal loads) it should be OK, but my preference is to avoid using inertial relief if possible.

[JonathanHodgson]

There are several ways to control this.

I like Shaun's symmetry constraint best. Symmetry is always good, where appropriate, because it makes the model smaller and therefore the run times shorter.

The key bit I think you've missed is:

"constrain each of the 3 cut surfaces such that they can't move in the normal direction defined by the surface."

Thus each surface isn't fully constrained: it's only constrained so that it can't move normal to itself. In this way, each surface is free to expand within its own plane, but between them they fully constrain the part.

A more general approach is one which I've heard called a "3-2-1" constraint. Using three vertices of the cube:

• The first vertex is constrained in X, Y and Z displacements - this prevents the part from displacing
• The second vertex is (ideally) positioned directly along the X-axis from the first, and constrained in Y and Z only - this prevents the part from rotating about Y- or Z-axes
• The third vertex is (ideally) positioned somewhere in the Y-direction from the first two, and is constrained in Z only - this prevents the part from rotating about the X-axis

[ptc-5675684]

Hi Jonathan,

Appreciate your help!

Following your guidance, I tried the "3-2-1" approach but no luck. Wildfire4.0 kept popping up warning:

"The highlighted point constraints can cause singularstress concentrations"

Now I am gonna attempt the symmetry approach....

Will keep you guys updated!

Lawrence

[JonathanHodgson]

Hi Lawrence,

Don't give up on that approach - the key words are warning (not error) and can (not will).

Let it run, and just satisfy yourself, by examining the results, that there are no unwarranted stress concentrations.

[sdensberger]

One thing to keep in mind about the 3-2-1 constraint is that your displacements are relative to the zero-displacement point; where this point is depends on how you set up the constraints.

[ptc-5675684]

Dear all,

I ended up using the Inertia relief to capture the stress and the result was validated by the symmerty approach.

The major mistake I made throughout the analysis was that I combined all plies into an advanced shell.

Now it has been fixed.

Thanks again for all the support and guidance!

Lawrence