Cosmosworks « Categories « SolidWorks Reseller Ohio, Kentucky, Indiana

Archive for the ‘COSMOSWorks’ Category

Beam Elements in Simulation

Wednesday, December 21st, 2011

One of the things that we emphasize in our Simulation Training classes is simplifying the model. It’s an easy concept to understand – the simpler the model, the faster you’ll get results! For designs that use SolidWorks’ weldment functionality, Simulation will automatically make one of the most significant idealizations of a model. 3-D geometry is idealized into a 1-D finite element for the mesh, a Beam element.

Here is a simple example where two standard c-channel structural members come together at what could become a welded joint (left side). Notice how Simulation has automatically meshed the structural member with beam elements (right side)! In Simulation 2012, you now have the option to render the beam mesh on the structural member geometry – a welcomed enhancement!

In Simulation, the purple spheres represent the ‘joint’ where the two or more beams are connected. There are also options for each beam’s end condition –rigid connection, hinged connection, etc.

How should you handle the automated power of Simulation with weldments? I say ‘handle with care’! Let’s assume that you have one of these c-channels as a simply supported beam – fixed at one end with a load applied at the other. The standard, cantilever beam that we all know and love from our Engineering studies! Recall that the deflection of the end of the beam is calculated by the following equation:
Deflection = (F * L^3) / (3 * E * I)
Where F is the force acting at the end of the beam, L is the length of the beam, E is Young’s Modulus for the beam material and I is the Moment of Inertia for the cross section of the beam.

This is valid, assuming the beam has a uniform cross section throughout its length. What if there are holes cut through the beam? In this scenario, the cross section of the beam is not uniform throughout the length – which is a critical assumption for the deflection of a simply supported beam. In this scenario, Simulation does not recognize the holes and still meshes the structural member with a Beam element.

In my opinion, you have two options for proceeding with the analysis. The first option is to recognize that using a Bea for the structural member is not an accurate representation of the model, but proceed with the analysis to obtain a baseline result. If this particular structural member does not significantly contribute to the overall strength of the model, you may choose to proceed based on these results. The second option would be to treat the structural member as a solid body. With this method you will obtain more accurate results with your analysis, especially if the structural member contributes to the overall strength of the model.

So the next time you’re reviewing your analysis results, be sure to review the assumptions made by both you and by Simulation. Once you’ve verified that all of the assumptions are valid, or at least that you can accept them, you will be well on your way to making sound decisions based upon your Simulation results. Now go make your products better with SolidWorks Simulation!

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Tags: Beam Elements, Bill Reuss, Meshing, Simulation
Posted in 3D CAD, COSMOSWorks, Simulation, SolidWorks, Tips & Tricks, Training | No Comments »

Fatigue Check Plot

Monday, November 14th, 2011

Should you be concerned about fatigue? Not the kind of fatigue that affects Air Traffic Controllers, but the kind that causes a product to fail after repeated use. If you have the luxury of designing products that are only used once, you can stop reading now! For the rest of us, we need to be aware of the expected service life of our designs. If you knew your product would last “forever”, would you run around the office high-fiving your co-workers? In Simulation Professional and Simulation Premium, we have a simple tool to quickly evaluate if your product can have an ‘infinite’ life. The tool is the ‘Fatigue Check Plot’.

Fatigue is the localized structural damage that occurs due to cyclic loading conditions. Fatigue also has cumulative effect on a structure – once damaged, always damaged. If the loads applied to the structure are high enough, microscopic cracks will appear on the surface of the part, eventually leading to a failure. Knowing the loading conditions (and, thus, the stresses that occur in the structure) and the number of expected cycles the product will see during its lifetime allows us to determine if our product is safe for the expected life of the product. If the stresses are high, the number of loading cycles the product can withstand are reduced. If the stresses are low enough, the product will have ‘infinite’ life. This stress level is usually referred to as the fatigue limit or endurance limit – a stress level that can act on the material without causing failure due to cyclic loading.

After conducting a static analysis study on the design, right-click on the Results Folder and select “Define Fatigue Check Plot”. The Fatigue Check Plot will be available if the static analysis used solid elements, shell elements or a mixed mesh with solid and shell elements. The calculations for a Fatigue Check Plot are based on an infinite number of constant amplitude cycles (loading events) acting on the product. Let’s take a look at the typical Fatigue Check Plot setup.

When creating this plot, there are several options. Under ‘Modifying factors’ the first is the loading type. You specify ‘ON/OFF’ loading, where the loads are applied and completely removed or ‘Fully reversed’ loading, where the full load is applied in nominal and reversed polarities. The second option is the Surface Finish Factor – surface finished can positively affect fatigue life (shot peening) or negatively affect fatigue life (electroplating). The third option is Loading Factor where you are specifying the loading type the material is experiencing; axial, bending, torsion, etc. The ‘Material’ section of the Fatigue Check Plot property manager allows for additional control of the results. You can enter values from 1 to 100 for ‘Scale this value’ and values from 1 to 10 for ‘Minimum safety factor’. ‘Scale this value’ multiplies the fatigue strength of the material by the scaling factor entered. ‘Minimum safety factor’ divides the fatigue strength of the material by the factor entered. Finally, what’s really nice is the preview of the results during the setup – for the (finished) plot above, we see the green check mark for the selected options and the caveat that you probably do not need to be concerned about fatigue in this design.

In this second plot, I have modified the loading conditions from ‘ON/OFF’ to ‘Fully reversed’ and obtain a warning that the design may possibly fail due to fatigue. I also receive the suggestion to run a complete Fatigue Analysis study on the design. Areas of concern on the part are shown in red on the finished plot.

So the next time you are wondering if your product will last forever, create a Fatigue Check Plot as a first step in analyzing the fatigue life of your design. If your initial results for a Fully Reversed, As Forged, Torsional Loading with a Minimum Safety Factor of 5 is in the green, take that victory lap and high-five your co-workers! Now go make your products better with SolidWorks Simulation!

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Tags: Bill Reuss, Endurance Limit, Fatigue, Simulation, Stress Analysis
Posted in 3D CAD, COSMOSWorks, Simulation, SolidWorks, Training | No Comments »

Material Properties in Analysis

Wednesday, October 12th, 2011

Have you ever considered the importance of Material Properties to your Finite Element solution? What about the accuracy of the data provided by material vendors? As Designers and Engineers, we are used to dealing with tolerances. We usually provide default tolerances on our drawing title block. We may add tolerances to some of the model dimensions. For the really bold and daring – or wise and experienced – you might even add Geometric Dimensioning and Tolerancing to your designs. Do you ever see tolerances on material property data sheets? In my experience, the answer is somewhere between rarely and never, with never in the lead.

Let’s consider a material from the Simulation material database. Alloy Steel has the following properties (numbers rounded):
Young’s Modulus – 30 x 10^6 psi; Poisson’s Ratio – 0.28; Mass Density – 0.278 lb / in^3; Yield Strength – 90 ksi

What will happen to the Finite Element solution if one material property varies? I’m going to start with a simple model in tension and apply Alloy Steel as the material using the default property values. Then I will change Poisson’s Ratio and re-run the study several times in order to compare the displacement and stress results. Recall that Poisson’s Ratio is a measure of the lateral strain to longitudinal strain for a material, or E_lat / E_long (pretend the E’s are Greek epsilon’s). Poisson’s Ratio is relevant to the linear elastic portion of the stress-strain curve and is unitless. One thing to note, if you do not define Poisson’s Ratio for a material, Simulation will assume that Poisson’s Ratio is equal to zero. There is a pop-up warning, too, just in case you forget to enter a value. Note that if you do not have Poisson’s Ratio for a material, 0.3 is a good initial estimate. But definitely exercise all of your options to find out the correct value for your design materials.

For a ½” square bar, 4” long, I have fixed one end and applied a 10ksi force at the opposite end, putting the bar in tension. After running the analysis with default material properties, I set a baseline with Trend Tracker. After creating several custom Alloy Steel materials, varying Poisson’s Ratio from 0.0 to 0.5, I re-run the analysis with each custom material. Trend Tracker will record the details for maximum displacement and stress in the model.

As you can see from the chart, the Von Mises Stress results vary approximately 16 ksi and the displacement results vary 0.00006 inches. As percentages, this is a 28% variation in stress and a 1.2% variation in displacement. I don’t think most of us would be concerned with 1.2% variation in our models, but 28% is an entirely different matter! I did, however, choose the model with this purpose in mind. The high stresses are at the fixed end at the sharp corner – something most Engineers would avoid in their designs. Now that a 28% variation has your attention, let’s look at a more practical model.

This is a simple bracket, a modification of a part in the SolidWorks Essentials manual. I’ve applied a fixed boundary condition to the bolt holes in the base and a normal force to the counter bore face. I’ve repeated the rest of the analysis, just like the square tensile bar, including using Trend Tracker and varying Poisson’s ration from 0 to 0.5.

For this “practical” model, the Von Mises Stress results vary approximately 4,300 psi and the displacement results vary 0.0006 inches. The percent variation in this model is 5.8% for stress and 6.6% for displacement. If you’re designing for a large Factor of Safety, less than 6% variation in your stress results are not significant. Using SolidWorks Simulation, however, most of us are designing for the lowest acceptable Factor of Safety in order to save the maximum amount of money possible on material costs. In this scenario, a 6% variation can be significant!

So the next time you’re analyzing that awesome design, consider reviewing the sensitivity of your analysis by varying a material property or two. Now you’re armed with powerful information you can share in your next design review. Material property variations from your vendors are no longer an issue! Now go make your products better with SolidWorks Simulation!

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Tags: Bill Reuss, Material Properties, Simulation
Posted in 3D CAD, COSMOSWorks, Simulation, SolidWorks, Tips & Tricks | No Comments »

Should I Flow with a Recommendation for CFD?

Wednesday, September 28th, 2011

It is interesting to note that the notion of complexity created by past CFD users is gradually getting replaced by a new era of acceptance and willingness to dabble in it. Of course, most of these early adopters are considered exceptions to the rule, and quite probably outcasts. However, they are probably not speaking out enough because they no longer have the time to speak out. Business is booming for them because they have products that are superior. They really have no more time!

Louver Model

CFD in the present age is a blessing well disguised. It hides behinds the curtains, on the monitors of a select few individuals who sit in those dimly lit cubicles in the corner of the office. For the most part, it is nothing but a blip on the screen – a process in the task manager, where no-one sees its burden rate. However, what has changed is its presence in the 3D world. With models flying around faster than the internet took over the universe, the traditional nerdy CFD specialist has been replaced with an engineer with a little extra time in his hand.

The neat thing about the product is that it speaks for itself. 3DVision recently did a consulting project for a customer on an industrial application. The model in question was moving air at a very high volume rate, and was encountering numerous obstacles on its way. Upon solving their model using Flow Simulation inside SolidWorks, we presented the results live in front of their management and engineering audience. As we approached the summary of results, one of the management members commented – “What you have shown us is an MRI of our design. In the past two hours, you have provided us with answers to questions that we have been raising internally over the past 2 years about the integrity of the design and its performance.” Such is the power of the software! This customer went on to purchase the software, and get trained in it. They are currently attempting at replicating the same workflow that we had adopted, on a different but similar model.

From concept to completion - Fluid flow around a Seascooter

The beauty of concurrent CFD tools like Flow Simulation is its versatility. While being extremely powerful functionality wise, it can be easily adapted to virtually any industry – valves, Industrial regulators, electronics equipment, medical devices, HVAC applications, commercial gen-sets, automobile drag and lift, and so forth to name a few. The underlying theme is the same – define the properties of the fluid, its inlet(s) and exit(s) locations, add any heat generation sources, create a mesh, and solve. And to top it off, the software gives the user the luxury of viewing results real-time to make any changes necessary right inside the SolidWorks graphical interface!

It would be noteworthy also to investigate the cost of not doing CFD, especially when the application involves moving fluids. In a recent study done by the Aberdeen Group (click here to read the post), the author identifies the top business pressures that force companies to investigate virtual simulation, and the leading impacts of not using CFD. The article underscores the need for companies to approach CFD with an open view and showcases how virtual simulation can very quickly become an integral part of product development.

exchanger

An important cog in the wheel of decision making has to be implementation. Not installing the software, mind you, but on learning how to use it, and getting good at it. I always tell my training class attendees that as easy as the software is, learning it is not an overnight skill. But the moment you digest the methodology and adopt it as a necessary step in your design evaluation, the benefits are enormous. Furthermore, it is so easy to customize it. For example, a customer of ours in the valve industry was adjusting their current design to meet a certain flow coefficient (Cv), a design requirement. Their methodology was to tweak a few variables, and perform a bench test. They went through 8-10 prototypes to get to the final model. Upon investing in Flow Simulation, they were not just able to run multiple iterations simultaneously and digitally prototype in minutes and hours, but were also able to create custom goals (an equation goal that determines Cv, and graphs it out for each run). Such equations can be created to monitor any parameter, such as efficiency of designs, maximum heat on components, drag coefficient values, etc.

So the next time you find that your fluid-filled product is failing in the field, or better yet, you are developing a new concept that needs some validation, be sure to examine Flow Simulation. Its needs are few, the benefits endless!

Vik Vedantham, Simulation Product Manager
Vik Vedantham
Simulation Product Manager
3DVision Technologies

Posted in COSMOSWorks | No Comments »

Solver Selection – Does It Matter?

Wednesday, September 14th, 2011

Choices. Everyone wants choices. We make simple choices like ‘paper or plastic’. Or one of my favorites, ‘domestic or import’! In SolidWorks we can be faced with decisions like ‘assembly or multi-body’! While these are simple examples, what do you decide when you’re faced with the decision ‘FFEPlus or Direct Sparse’? Which solver should you select? While this question does not have an easy answer, there are some guidelines you can follow to help in your selection. Understanding the two solvers is the first step in making a smart decision about which to use.

Before discussing the solvers, let’s recall the fundamental equation being solved by Finite Element Analysis, which is the resultant forces acting on a body are equal to the product of the stiffness and resultant displacement of the body. We express this with the following matrix equation: [F] = [K] * [U]. Regardless of the solver selected, this equation has to be calculated such that equality exists.

The FFEPlus solver is an iterative solver. After you have the CAD model set up with the appropriate boundary conditions, the FFEPlus solver makes an educated guess about the deformation, [U], of the model. Then it evaluates the matrix equations to see how good the guess was, and adjusts the deformation accordingly, depending upon the error in the calculation. This process repeats until the calculation balances.

The Direct Sparse solver is just that – direct. This solver will create the entire matrices used for the numerical FEA solution. This requires generating the stiffness matrix, [K], as well as the inverse of the stiffness matrix, [K]-1. Once calculated, Direct Sparse solver has to compute a simple multiplication problem, written out as: [K]-1 * [F] = [K]-1 * [K] * [U]. Computing the inverse of the stiffness matrix is resource (memory) intensive.

Now that you know what the solvers are, let’s discuss and compare the two solvers, at least as far as how they may relate to your Finite Element Model. If your problem has 25,000 degrees of freedom (DoF) or less, the Direct Sparse and FFEPlus solvers are approximately equal in terms of memory usage and solution time. For problems that approach 300,000 DoF, the Direct Sparse solver usually runs entirely in your system’s RAM, which provides for a “fast” solution. When you exceed 300,000 DoF, the FFEPlus solver is more efficient than the Direct Sparse solver in not requiring as much of your system’s RAM. There are times, however, regardless of the problem size that you may need to use one solver over another. In assemblies with a lot of contacts, assemblies with greatly varying material stiffness between components and contacts with friction, the Direct Sparse solver is usually a better choice. In frequency studies with Rigid Body Motion and problems exceeding 300,000 DOF, the FFEPlus solver is usually the appropriate choice.

What do you do now? You know what each solver is doing at the core. You have a general understanding of what each solver is good at. How do you decide? It’s actually a very simple answer – let Simulation decide for you! In SolidWorks Simulation, there is a system option to let the program decide. To access this, from your pull-down menus, select “Simulation… Options…”, then change to the “Default Options” tab and click on the line for “Results”. Then look at the section for ‘Default Solver’ – we have ‘Automatic’, ‘Direct Sparse’ and ‘FFEPlus’. Set your Simulation system options to ‘Automatic’, and let SolidWorks Simulation decide which solver is the most appropriate for your Finite Element Model. With that decision made for you, you now have time to make your products better with SolidWorks Simulation!

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Tags: Bill Reuss, Direct Sparse, FFEPlus, Finite Element Analysis, Simulation, Solver
Posted in COSMOSWorks, Simulation, Tips & Tricks | No Comments »

Model Aircraft Control Surface Spacing and SolidWorks Flow Simulation

Saturday, August 27th, 2011

June 2011 AMA (Academy of Model Aeronautics) Model Aviation magazine had an interesting article Titled “Two of the Big Five model misadjustments” written by Dean Pappas. The two misadjustments were Hinge Gap, and Lateral Balance.

The article caught my attention specifically due to the “flow” diagrams drawn in the article explaining airflow over the wing section and aileron control surface. In the below diagram, taken from the article, Dean explains three cases of air flow relative to a control surface.

Clean airflow at the neutral control surface desired for level flight.
When up or down direction is applied to the control surface the air opposite the control surface direction of travel redirects the flow to reattach. This case shows a tight fit between control surface and main structure.
Hinge gaps allow high-pressure air to leak from one side to the other. This weakens airflow on top of control surface partially destroying the bottom airflows ability to rejoin it. The result is poor control surface response during slow speeds.

AMA Article Diagram

According to the article ”The high pressure on top, as shown would leak through, given a chance. That chance would be a gap in the elevator and control surface. The result is a flat sheet of air that squirts through the gap and distorts the outside of the hinge line. This reduces the effectiveness of the elevator and creates extra drag.”

This section piqued my interest as the hinge gap shown is very large, probably for demonstration purposes. Being an avid RC aircraft modeler I suspected that the small gaps I have in my personal aircraft’s control surfaces may not cause this affect. My hypothesis is that a very large unrealistic gap will cause this affect however using standard hinge techniques this affect will not be as dramatic as the article states. According to the article large hinge gaps can be sealed with strips of MonoKote covering resolving the problem. MonoKote is a heat shrink Mylar covering that is a standard in RC Aircraft construction.

This blogs purpose is to investigate the hinge gap spacing required to cause an airflow disturbance and air leak through the gap area.

Before we get into the model specifics let’s talk a little about aircraft wing terminology. Below is a diagram explaining common wing dimensions and terminology. The chord length is the distance from the leading edge of the wing or elevator to the trailing edge. The model used in this Flow Analysis is a 5.5″ main wing chord. 0.5″ of the chord is the control surface . The airfoil is symmetrical so the upper and lower camber are equal. The model consists of an extruded wing section with one hinge placed in the middle of the wing.

Three hinge types are standard in the RC modeling community. All hinges are typically spaced evenly across the control surface.

Standard plastic barrel hinge comprised of two halves held together with a pin. The hinge is typically screwed or glued into place with the barrel tight against both mating sections. Hinges are typically 0.25″-0.5″ wide by 0.5-1″ total length. The barrel typically ranges from 0.0625″-0.125″ in diameter.
CA hinges are flat woven wicking material that is inserted into a slot cut in the components. No or little gap is present with this style hinge. CA or Cyanoacrylate glue is used to wick through the hinge and bond with the hinged components.
MonoKote hinges are seldom used in modeling except for small aircraft. The MonoKote hinge is typically a strip of MonoKote that is applied to the top and bottom of the hinge area.

SolidWorks Flow simulation was used to investigate the control surface configurations of four models.

A base line neutral control surface position using a no gap CA hinge Type.
Upward deflected control surface using a no gap CA hinge type.
Upward deflected control surface using a Standard plastic hinge with an 0.0625″ barrel diameter.
Upward deflected control surface using a CA Hinge and gap of 0.25″

All configurations have a 10 ft/second flow rate and a 0 degree angle of attack. The flow analysis was an external flow problem. A localized mesh control was used for each run to capture refined accurate results across the model boundary. All other default conditions were used for the flow setup.

Mesh

Note All plots show a Pressure cut plot and Velocity Flow Trajectories.

Results:

The base line model showed a symmetrical pressure on either side of the wing at 14.6 psi and a hinge crossing velocity of 16.45 ft/sec. This is expected results for the area section, hinge, and aileron placement.

Neutral Velocity and Pressure

Flow Run Two shows a higher pressure on top of the aileron of 14.696 psi and a lower pressure on the bottom of 14.694 psi. The flow velocity across the top of the control surface drops to 5.9 ft/sec while the bottom speeds up to 11.2 ft/sec. As the article states the air “bends” to re attach to the flow at the trailing edge. This results in a turbulence on the bottom of the control surface aiding in the force of the air on the top of the control surface to push the trailing edge down.

Aileron Up CA Hinge

Flow Run Three demonstrates the 0.0625″ barrel hinge gap and the resulting air flow. The run does show airflow across the gap boundary, however probing the area the velocity in this gap is zero. The flow does extend past the wing trailing edge longer than the non-gap position, however the flow does fully rejoin. The same recirculation under the control surface is seen . The pressure on the end of control surface is however higher at 14.699 psi and lower on the bottom at 14.692 psi. The results show negligible flow through the gap and under most circumstances(slow flight) should not cause loss of control due to bleed through.

Aileron Up 00625 Gap

Run Four had the largest gap similar to the gap in the article’s diagram. The flow results show airflow across the gap boundary and a velocity of the airflow in the gap of 3 ft/sec. The flow does extend past the wing trailing edge longer than the non-gap position and does not rejoin. The recirculation does cause a pressure equalization under and over the control surface. Loss of control surface effectiveness would occur in this scenario.

Aileron Up 025 Hinge Gap

Conclusions: The article is correct to a point. The gap shown in his diagram would cause a control surface loss of effectiveness, however the gap is way too large to be considered realistic. Most experienced modelers know common practice is to get as tight of a fit between control surface and structure be it a wing, elevator, or rudder. A large gap is not only detrimental but is also unsightly and most modelers avoid them for the aesthetic reasons alone. If a modeler sticks to the new CA hinge or follows correct installation practice for a plastic hinge they will be alright in their flying endeavors.

Robert Warren Application Support Engineer CSWP / CSWST / CSWI / CSPS 3DVision Technologies

Tags: Academy of Model Aeronautics, Aileron, AMA, Dean Pappas, Flow Over Airplane Wing, Hinge Gap, Model Aviation magazine, RC Plane, Robert Warren
Posted in 3D CAD, COSMOSWorks, Case Studies, General, Simulation, Tips & Tricks, Training | 1 Comment »

Convert Durometer to Young’s Modulus

Thursday, July 14th, 2011

If you work with rubber and plastic materials frequently, you more than likely have access to a stress-strain curve for use in Simulation. What can you do, though, if you don’t have all the required material properties for analysis? If you’ve ever searched for material properties via MatWeb, IDES or other sources, you’ll likely find the hardness of plastics and rubbers listed in Shore-A or Shore-D – and no Young’s Modulus. Fear not! There is a simple calculation to convert a Shore durometer to Young’s Modulus, which is sufficient to get you started with your analysis work.

Before I show you the calculation, you should be aware that there is not a direct relationship between a Shore scale and Young’s Modulus! The calculation allows you to approximate ‘E’ based on a range of Shore-A (20 to 80) or Shore-D (30 to 85) durometers for simple static analysis.** If you routinely work with plastic and rubber materials, you should be using SolidWorks Simulation Premium with the actual stress-strain curve for the material(s) you design with!

For a durometer given in Shore-A, multiply this value by 0.0235. Then subtract 0.6403 from this result. The next step is to find the inverse base-e logarithm of this new result. The answer is an approximation for Young’s Modulus in megapascals (MPa). To convert this to pounds per square inch (psi), simply multiply this number by 145.0377. If you’re like me, word problems were never a strong suit! Here are the equations to input into Excel for a Shore-A or Shore-D durometer – or download the Excel spreadsheet here.

Shore-A to Young’s Modulus (in MPa):
=EXP((Shore-A Durometer)*0.0235-0.6403)

Shore-D to Young’s Modulus (in MPa):
=EXP((Shore-D Durometer + 50)*0.0235-0.6403)

Replace the ‘Shore-A Durometer’ or ‘Shore-D Durometer’ with either a number or the cell location of the value.

** Making Engineering decisions based upon analysis results with this “material property conversion” is not recommended.

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Tags: Bill Reuss, conversion, Durometer, Excel, Simulation, Young's Modulus
Posted in 3D CAD, COSMOSWorks, General, Simulation, Tips & Tricks | No Comments »

Dimension Printed Simulation Verified Blow Off Valve Adapter

Wednesday, June 29th, 2011

Adding a new Blitz Blow Off Valve (BOV) to an aftermarket turbo system lead to no clearance between the valve and the hood of the vehicle. An adapter was needed to drop the BOV from the high pressure pipe outlet to between the twin cooling fans behind the radiator.

High Pressure Pipe Assembly

BOV Adapter

The problem statement is as follows:

A custom adapter was developed to accommodate hood clearance. Before final fabrication out of aluminum a prototype was “printed” using a Dimension Rapid Prototype Printer. The printed ABS parts are inherently porous and needed to be sealed in order to hold pressure. The part was dipped quickly in acetone and then washed thoroughly with soapy water to seal the pores. The part was then tested to 110 PSI on a test bench before failure. A second part was then tested on the car.

Because operating pressure is only 10 PSI, a FOS of 10 was provided by the design.

110 PSI Failure

The second consideration is that the BOV is cantilevered off of the high pressure pipe bung . The BOV weighs approximately 1/8th of a pound. Adding this to the loading still produced a FOS of 5.

Combined Load

Simulation verified the physical test results and showed that the printed part holds up to the design requirements. The printed ABS adapter works so well an aluminum version was never fabricated. 110 passes down the 1/4 mile drag strip, 1000’s of miles, and 4 autocross seasons, and the little plastic adapter keeps on going.

Robert Warren
Application Support Engineer
CSWP / CSWST / CSWI / CSPS
3DVision Technologies

Tags: Cosmos, dimension, Printing, Robert Warren, Simulation, SolidWorks
Posted in 3D CAD, COSMOSWorks, Dimension Printing, Simulation, Uncategorized | No Comments »

Design Changes To A Popular Bath Toy Using Simulation Premium

Tuesday, May 31st, 2011

Recently for his 1st birthday my son received an interesting bath toy. The toy has an electric pump that flows water from the bathtub out the spout through a suspended set of cups. One of the cups funnels the water to a spinning wheel. The other disperses the water through small holes, and the last has a floating center that rises as the water collects in the outer cup.

Bath Toy

What I noticed is that the plastic arm that suspends the cups under the water flow may require a design change. The issue arises due to repeated addition of force in the arm from my son. Although the arm is plenty sufficient to hold the plastic cups as designed it is not equally as designed for a 1 year old to repeatedly pull down on the end of the arm to remove the cups. Repeated addition of this force has caused plasticity in the arm at the connection to the base.

Let’s examine the geometry to better understand the issue.

The larger ring accepts the cups. The arm runs between the large ring and the small ring that mounts to the inlet shaft. A small fillet is used to blend the interface between the arm and the small ring. In my opinion this fillet is too small. Here’s why. Stress = Force / Area. The smaller the area (fillet size) the higher the stress.

The arm was modeled reconstructing the dimensions using caliper and a scale. Note the dimensions are approximate.
The first model has the original fillet size.

Modified Geometry

As a design change the second model has a larger fillet added to distribute the stress.

Original Geometry

The model material was assumed to be ABS standard with the SolidWorks Library. A more accurate material definition is needed for any real design changes to be recommended.

The problem statement is as follows:

My son takes a bath every night. On average the arm is bent 4-5 times during the course of the bath. Based on the one month the toy has been in use 30 X 4.5 = 135 applications of force applied so far. I will analyze the existing and the proposed geometry for stress based on a specific displacement. Next perform fatigue analysis on the existing and proposed design for the arm.

The arm is fixed at the recessed ledge where the collar meets the inlet shaft. A specified downward displacement of 1.75″ based on my sons actions is applied to the outer most portion of the large ring.

Due to large displacement in the model and the nonlinearity of the material Simulation Premium was used to analyze the geometry. Note the material specifications are not exact and a generalized S-N curve was used for the fatigue analysis. A zero based loading was used for fatigue.

Results:

Original Design Showed 20000 PSI of stress at the fillet area.

A fatigue life of 890 cycles for the same area.

Stress Large Fillet

Original Design Fatigue

The modified larger fillet showed much improvment Stress of 10000 PSI and a fatigue life of 4000 cycles.

Stress Original Design

Fatigue Modified Design

If the geometry is modified with a larger fillet the toy will be enjoyed a great deal longer. From the design change a life of 4000 cycles, my son will be 4. Before then, I am sure it will be passed on to a little brother or sister.

Robert Warren
Application Support Engineer
CSWP / CSWST / CSWI / CSPS
3DVision Technologies

Tags: 3DVision, 3DVision Technologies, Robert Warren, Simulation, SolidWorks, Tips and Tricks
Posted in COSMOSWorks, Simulation, Uncategorized | 3 Comments »

Mesh Failure Diagnostics, Part 2

Monday, May 16th, 2011

Last month, I wrote about Mesh Control and described a process using the Simulation Advisor to fix mesh errors. If you prefer to operate without the proverbial ‘phone-a-friend’ option, you can always turn the Simulation Advisor off by un-checking the box in your Simulation Options, as shown. When you uncheck this box, you still have the option of accessing the Simulation Advisor from the Command Manager by selecting the appropriate Advisor in the pull-down menu.

When an assembly failed to mesh in Simulation 2010, you had to know your assembly components well to determine which part(s) failed to mesh. Recall that the Simulation Feature Tree looked like this:

With SolidWorks Simulation 2011, however, we now have a visual indication for which parts failed to mesh in the Simulation Feature Manager Design Tree. Notice all of the component icons that are colored red? Simulation 2011 provides this visual feedback to let you know where the mesh failures occurred. If you right-click on any of those parts and select ‘Create Mesh’, this will start the Mesh Control dialog for the selected part. Apply a mesh control and click ‘OK’ to mesh the part. Using this method, you have to apply mesh controls to a single part at a time. If you control-select several of the red (failed) parts from the Simulation Feature Manager Design Tree, you need to right click on the Mesh folder and select ‘Apply Mesh Control’. Note that when you choose this method, you will need to recreate the mesh for the entire assembly.

Bill Reuss, CSWE
Application Support Engineer
3DVision Technologies

Tags: Bill Reuss, Mesh Control, Meshing, Simulation
Posted in 3D CAD, COSMOSWorks, General, Simulation, SolidWorks, Tips & Tricks | No Comments »

Archive for the ‘COSMOSWorks’ Category

Beam Elements in Simulation

Fatigue Check Plot

Material Properties in Analysis

Should I Flow with a Recommendation for CFD?

Solver Selection – Does It Matter?

Model Aircraft Control Surface Spacing and SolidWorks Flow Simulation

Convert Durometer to Young’s Modulus

Dimension Printed Simulation Verified Blow Off Valve Adapter

Design Changes To A Popular Bath Toy Using Simulation Premium

Mesh Failure Diagnostics, Part 2

Recent Posts

Categories

Pages

Archives