Imaginary Materials

Originally published in 2009

In the world of FEA, sometimes the answer has to be “Right” – and sometimes it has to be “Right Now”.
This month’s topic is about getting answers Right Now. Every example I’m going to cover here is a cheat of some kind. Purists, Beware! In each of these examples, the key to the method is to invent imaginary parts on which to apply loads or restraints, or imaginary material properties, or both. These materials will sometimes allow us to avoid computing real-world Gap/Contacts, or will turn a marginally unstable problem into a stable one, or will allow us to use a force-based load where a deflection-based boundary condition would be too confined.

Cheating Contact Problems with “Softium”

Simple snap-fit hookPictured at left is a simple, idealized model of a snap-fit hook. The goal of the analysis is to determine the stresses when the geometry is depressed by 2 mm in order to catch in a slot in an outer wall. This is going to require a Large Deflection solve. How to set this up?

The “Real” solution would be to set up a Contact problem. A sliding contact on the outer tip of the hook will allow you to enforce the 2 mm depression, but would otherwise not over-constrain the hook, leaving it free to rotate as it undergoes a classic beam deflection. Unfortunately, Gap elements are very, very slow to compute. But, let’s look at that formulation first, as a baseline for our stress and deflection.

For this formulation, we need very little of the wall solid, really just the ramp surface, as shown below. We solve this as a constrained-deflection problem, forcing the ramp body to slide 6.5 mm to the right. The Solver options used are “Large Displacement”, and “Direct Sparse”. The 6.5mm deflection was measured carefully – we do NOT want to push the ramp past the point of ‘snapping’ back up, because that would be a point of instability (zero-stiffness).

The resulting peak stress is about 5700psi, and the solver took about 9 minutes to run this simple problem.

Resulting stress analysis on snap-hook

Now let’s look at the simplest possible problem formulation, one that avoids using any Contact elements. It is tempting to simply apply the desired downward (-Y) deflection directly to the top face of the hook. But this boundary condition would create artificial secondary stresses in the hook, because the restraint would limit all nodes of the face to the same relative Y translations, effectively forcing the face to move parallel to itself. This is wrong, of course – we know that the hook should experience some rotation as well.

The image shows that the Y-only restriction on the top face of the hook

The image above shows that the Y-only restriction on the top face of the hook, is artificially applying a torque to the end, in the reverse of the direction that the hook should be rotating. Compare this image with the first result on the previous page – this run lacks a clearly-defined neutral axis (Blue stripe along the mid-thickness) due to bending. What this result has, instead, is a dark blue stripe transverse to the hook bend direction, and this shows an inflection in the shape. Ignoring the peak stress at the point of load application, we see that the stresses back at the root of the hook are reporting higher, around 7000 psi, compared to our baseline run with Contact. It did at least solve quickly, taking about 80 seconds. Too bad it is wrong.

So here’s the “Softium” trick. Create a block of material to push down on the end of the tab. This body should be made out of a very soft, rubber-like material, with a stiffness less than 1/10th that of the hook material, (I used 8000 psi), and the Poission’s ratio should be close to rubber, I usually use .485. (Don’t get too close to a Poisson’s ratio of 0.5, as this would be purely incompressible, and would cause solver stability problems).

You want the block to be as thin as possible, so that its elasticity does not throw off your computed deflection too much, but you do want 2 mesh nodes thru the thickness, to allow elements to displace laterally and rotate where in contact with the hook. Notice the image below, where the peak stress at the hook root is now around 5900 psi, and there are hardly any stress concentrations due to torsion out at the tip. This result took less than 2 minutes to compute.

By probing the hook top, we learn that it only deflected downward 1.95mm, because the presser-block absorbed some of the deflection. But, we can now re-run this study with a Y deflection of 2.05mm to compensate, and we will still have our results faster than having run the full-contact study. As the contact problem gets larger and more complex, this technique can save you hours of compute time, and still get you very close to the true stresses.

KAP’s Tip: After adding new Parts or Bodies to an FEA problem, use Update All Components so that Simulation will add the new Material folders

Springy Foundation Pads

Now let’s consider the simplest of all problems. The beam at left is anchored in a wall, with a tensile load of 2000 lbs, and has a cross-section of 2 square inches. If you use a simple FIXED restraint on the left face, this removes all degrees of freedom from the mesh nodes. But this not only keeps the beam from pulling out of the wall, it also keeps the beam width and height from ‘necking down’ to comply with Poisson’s effect. Because the last row of nodes are thus artificially un-compliant, but the next row of nodes inboard of the end can comply with Poisson’s effect, the stresses at the corner elements are way above 1000psi because of the added shear strain, (see image below).

We know to ignore these stress results as an artificial by-product of the mathematics of the restraint. But what if the peak stresses in the vicinity of a restraint are actually significant to the problem? Let’s first look at a couple of the ‘standard’ techniques.

Solution 1: Soft Springs.

Change the restraint at the wall to be “On Flat Face”, and allow zero motion in the “Normal to Face” direction. This only restrains the beam in the global X, however. To prevent accidental motion in Y or Z (due to round-off error in the solver, mostly), we turn on the solver property to use “Soft Springs” to stabilize the model. The resulting stresses are very close to our theoretical 1000 psi. In fact, if you look at the result plot below, especially look at the scale of stress magnitudes, and you see that the mottled blue-cheese appearance is really just a plot of round-off error – computer noise.

But Soft Springs can only be applied if there are no loads that would act in the unrestrained directions. And, for problems involving large-deflection, or contact cases, any rigid-body motion inherent in the problem will be altered by the soft springs trying to pull the model back to the start. In the example above, you see that Soft Springs have arrested the model from rigid-body motion, but not before it has drifted some from the origin, including mostly rotation. So soft springs are sometimes useful, sometimes not.

Solution 2: 3 Orthogonal Restraints Scheme

First, the anchor face is restrained only against motion “Normal to Face”, just like in the Soft Springs case. But then, select one of the vertical edges, and restrain against motion in the Z direction. And, selecting one of the horizontal back edges, restrain against motion in the Y direction. Now there is only one point in the model that is held against X, Y, and Z, and the rest of the anchor face can expand or contract under Poisson’s effect. This is my first choice of how to tackle restraining most FEA problems. But, it is still not perfect. Look at the stress plot below, for example.

In this example, I’ve applied not only the 2000 lbs tension along the length of the beam, I’ve applied a 500 lb downward force on the end to get some bending moment. Restraining the long vertical edge against motion left-to-right, and the top edge against motion up-and-down, does a great job of eliminating degrees-of-freedom – it is firmly pinned at the upper-right point. But consider the bending stresses – the top half of the beam is in tension, and so should neck down somewhat. And the bottom faces of the beam are in compression, so they should bulge outward some. So the vertical edge wants to rotate – but cannot. (If our beam were to have any lateral bending moments, then the top and bottom edges would want to rotate, too!). So, in the most general case, even this careful system of restraints is going to bias the resulting stress to one side or the other. And of course, you could apply a couple of Split Lines to bisect the end face, and put your 2nd and 3rd restraints on these interior seams, instead of outside edges. That would be better, but still presumes you know ahead of time where to sketch those lines, to align with the neutral-axis of bending…

All I’m trying to get at, is that pretty much any system of restraints is going to be a compromise between what is easy to input mathematically, and what is really going to happen to the deformed shape. So, here is my submission for a 3rd way to anchor a model face in space:

Solution 3 “Springy Foundation Pad”

Start by sketching on the face that you want to anchor. Use CONVERT to copy the edges of the face, and then extrude it to create an extension of the sketch as a separate body, (clear the “Merge Result” option). This will be your Foundation Pad. It needs to stay as a separate body for two reasons. We are going to give it a different material property from the beam. And, we need the contact face between the beam, and the pad, to remain as a distinct entity for applying a boundary condition. The pad should not be too thick, because we want it to mesh with only 1 row of elements, (see below).

KAP’s Tip: Any system of restraints is going to be a compromise between mathematical inputs and reality. So I suggest you anchor the model face in space with an imaginary springy foundation pad.

Next, set the Young’s modulus of the foundation pad to be low – maybe as low as 1/10 of the stiffness of the adjoining part. And, set the Poisson’s Ratio to be something really low – I usually use 0.1.

Now for the trick. Select the face that lies between the Foundation Pad, and the Beam, and restrain this face against any motion in only 1 direction – normal to the face. Now select the outside face of the foundation pad, and on this face, restrain against motion in the other two, in-plane directions. This is like creating your own custom “Soft Springs” option, only they will act only on the anchor face, not on any other face of the model. And, the low Poisson’s effect means that the Foundation Pad will transmit practically no shear stress back into the end of the model.

In the image below, we see the Elemental Stress patter that develops from this restraint system, when the beam is loaded with the same 2000lbs applied axially, and 500lbs applied downward, at the end. The springiness of the foundation pad has allowed the model base to shifted downward due to the shear loading, but this displacement is small, .00028” max. I use an Element Stress display here, because the Nodal stress plot, due to averaging, makes the stress appear to fall off continuously across the interface to the Foundation Pad, but you can see here that it clearly falls off immediately.

For those of you keeping score on the methods, Method 2, (3 Orthogonal Restraints), reported a peak elemental stress of 10,063 psi, but this stress peak was on one upper corner only, and the other corner’s elemental stress was 9,237 psi. The Soft Springs option can’t be compared, of course, because soft springs can’t resist the 500 lbs bending load.

Force-Loading with displacement limits

This final method is visually very simple, and is closely tied to a specific problem. I had to analyze a rubber tire, for both the amount of ‘give’ when under vehicle deadweight, and also the amount of grip the tread afforded when a skidding force is applied at the ground contact patch. But testing for slippage under skid-loading is tricky business for the solver. The loading at the axle will create a deformed shape of the tire, and the resulting footprint on the ground will create a variable pattern of contact stress with the ground. For any given skid-loading, some areas of the tread could be loaded heavily enough to ‘grab’ the road, and other areas will be so lightly loaded that slippage occurs. (This is why a tire can ‘squeal’ and still be holding the road). Each area of local slippage will look to the solver like instability, and of course if enough areas areas slip, and the tire completely loses grip, the skid force is then unopposed by anything, and the solver will halt. So getting the analysis to run to completion is touchy.

If only we could solve this problem using a Displacement-Control, instead of Force Control, it would behave much better. But, you probably already know that the Displacement Control option does not work for Contact problems. And I need to do a Contact study to see how much the rubber tread pattern is in contact with the road. So, how to stabilize the force-based problem?

This problem is solved by a system of three models; the tire, a plate representing the ground, and an imaginary material used as a spring to back-stop the ground plate if it slips, (shown in blue below).

ThemodelpThe model pictured above does not show the wheel rim or axle, where the vehicle weight-loading is applied, but I should mention that restraints on the axle will only allow the tire to deflect downward – ie., it cannot ‘roll’ along the ground. So when a force is applied to slide the ground under the tire, frictional contact with the rubber should prevent the plate from moving. If the rubber-to-ground friction is not enough and the plate would ‘slip’, it is backed-up by the blue material.

Assign this body a very weak spring constant, maybe 1/100 of the shear modulus of the rubber. That way, you can check the reaction force at the “Fixed” relation at the back of the spring-plate. The difference between the load applied in the front, and the spring reaction in the back, is how much braking force went into the tire rubber.


Because my own background is rooted in Manufacturing, when I think about a system of restraints for FEA, I tend to compare it to tooling jigs and clamping fixtures. Some tooling is ‘fixed’ – hard tooling that you intend to use again and again. Most of the Simulation “Fixtures” folder contains what I would consider ‘hard tooling’. But sometimes restraining a part in the machine tool is trickier, and you have to use “Soft Jaws”, which are sacrificial tooling. It is purposely much softer than the part, or the cutting tools, and so clamps the part more gently, and can be thrown out after use if the cutting tools need to run into it. In this KAP’s Corner, I’ve shown how you can apply the same thinking to FEA – clamp your parts in space, by designing tooling blocks with artificially soft material properties, and then put your ‘hard’ restraints on the outer faces of these blocks. You always sacrifice a little accuracy when you do this, but you gain in solution speed, and sometimes, stability.

Have a Solidworks bone to pick? Want more tips in a specific area of the CAD? Keith is looking for requests from users for future KAP Corner topics. Email your suggestions to; KAP@CAPINC.COM

KAP’s Tip: Use “Soft Jaws” to clamp your parts in space. This sacrificial tooling method can often speed up your solution time as well as provide stability.


CT | MA | ME | NH | RI | VT