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Posts Tagged ‘mates’

This is a very short post with the only intention of showing you a little video where I’m driving movement in an animation using only an angle mate. The video was also made made using SolidWorks 2010 Motion Manager and it’s the same model of the scissors that  I used before, but  it kind of didn’t fit well with the other two examples, so I decided to make a separate video about it. There’s also a little something on changing views during the animation. Hope you find it useful!

 

Hey everyone!  I know it’s been almost a month since the last time I blogged.  I also know quite a few of you still visit. Thank you!  Contrary to what the rumors may say, I’m still alive and this blog is still active, just not as active as before.  I’m sorry! Truth is this summer – this whole year – hasn’t been exactly one of the best ones for me and I’ve been seriously tied up with family responsibilities and other mundane activities. Bo-ring… I know.  Precisely for that reason I considered having a friend of mine as a guest blogger every now and then, just to keep the ball rolling during those times when I can’t come up with something to write about or when I just can’t find the time to do it, but he’s not convinced this is something he may want to do.  I guess I haven’t nagged enough.

As I mentioned a couple of posts ago, I’ve been reading the new book Creating Animations with SolidWorks and I’m already halfway through it.  At the risk of sounding like a bad commercial, I must say that this book is really worth the time and effort.  It is very easy to read, straight forward, and will quickly provide you with the tools you need to create really cool animations without complicating your life.  

I think one of the most important things I’ve gotten from this book so far is the understanding of what making an animation in SolidWorks is really about. You see, I started the process backwards, attempting to understand SolidWorks Motion first, before learning about animation, and I was confused because all three kinds of motion studies use the same interface: the Motion Manager, although they are definitely not the same thing . This book has helped me finally understand why many of my previous attempts failed, and find different ways to get the movement right.

I’ve learned that sometimes you may get the results you need by dragging parts, sometimes you may drive the movement using distance or angle mates and yet some other times you may use one or several motors to accomplish the same.  And you can combine these elements too! Reading chapter seven I learned how to apply motors, how to turn them on and off throughout the timeline, reverse their direction, change their speed,  and change the interpolation mode to affect the way they operate, thus ultimately changing the way the whole animation looks like. I also tried one kind of motor I hadn’t tried before in an animation: an interpolated motor, driven by a tabulated set of values. This sort of motor is pretty cool, because it’s easier than trying to keep track of several key points throughout the animation, especially if you have other motors that you are trying to synchronize.

Anyway,  I put something together really quickly, trying to answer the second question from the same reader of the chain. He wanted to know how to animate screws so it looks like they are actually being screwed or unscrewed during the animation of an assembly exploding or collapsing. I tried two different things, based on examples I found in the book.  If you want to know more, I recommend you get a copy of the book Creating Animations with SolidWorks from your local VAR or the SolidWorks online store.

For the first method, I created a manual animation of the explosion of a pair of scissors. By manual I mean that I didn’t use the Animation Wizard, but dragged and positioned the components myself, instead.  Notice that, in order to do this I had to suppress a few of the mates in the assembly or else the components wouldn’t budge at all.  For the second method, I used the Animation Wizard to create an animation of the assembly explosion first and then tweaked the animation a bit.  In both cases, the rotation of the screw was achieved by using a screw mate. Please, forgive me because these two animations are extremely rough. I didn’t pay too much attention to details and views, etc., so they may not look as nice as they could had I spent a little more time working on them. Anyway, to watch the video simply click on the image below.

I hope none of you minds this bilingual post. I still don’t really feel like resurrecting the Spanish blog, but this question was asked by someone who speaks Spanish, so I feel it’s only fair to give an answer in Spanish, as well.

Espero que a nadie le moleste que este blog  en particular sea hecho en forma bilingüe, pero la pregunta que lo inspiró fue hecha por alguien que habla español y considero justo que se le responda en español.

The question was about  doing an animation of a chain that is driven by a couple of gears, kind of what you would see in an engine or a bike. In fact, I think my reader is intending to do something very similar to what’s shown in this impressive video.

La pregunta que me hicieron fue acerca de cómo realizar la animación de una cadena de eslabones  conectada a un par de engranes, como las que se ven frecuentemente en algunos motores o en las bicicletas. De hecho, mi lector está tratando de hacer algo semejante a lo que se muestra en este impresionante video.

http://www.youtube.com/watch?v=6S__Fxpiccs&feature=fvsr

I also found a lot of other similar videos of chains and gears on YouTube, but sadly they were all made using AutoDesk Inventor. Anyway… While I don’t have the skills (or the patience) of whoever did that animation, I did come up with a way to  help my reader create something that is hopefully somewhat similar to what he wants to do with the chain using the Motion Manager in SolidWorks.

Además de este video, encontré algunos otros en YouTube, pero desafortunadamente  al parecer esos videos fueron hechos con AutoDesk Inventor, así que no me fueron de mucha ayuda. Bueno, quizá yo no tengo la misma habilidad ( o paciencia) de quien hizo esos videos, pero al menos pude generar algo que talvez le ayude a mi lector a realizar lo que desea usando el Gestor de Movimiento de SolidWorks.

I remembered that some time ago I had seen an animation of a chain in another blog called SolidWorks Unleashed. The author used a special type of mechanical mate called a cam mate to force the links in the assembly to follow a closed path he created using an extruded surface. I decided to do something similar to what he did. I think he mentions in the video that he’s mating to a point, but I can’t really see where the point is because the video is very blurry, so I used the cylindrical faces of the links as a mate entity for the follower, instead.

Me acordé que tiempo atrás  había visto una animación de una cadena de eslabones en un blog llamado SolidWorks Unleashed. El autor hizo uso de un tipo especial de relación de posición conocido como Cam (leva) para forzar a los eslabones a seguir una trayectoria cerrada que el mismo creo usando una superficie extruida de un croquis. Yo decidí hacer lo mismo que él. En el video él menciona estar utilizando un punto en el eslabón para designar el seguidor, pero yo no alcanzo a ver dónde se ubica ese punto, pues el video es muy borroso, así que use las caras cilíndricas de los eslabones en su lugar y funcionó bien.

OK, so the first step was to create a path for the links to follow. I started with the assembly of gears that my reader sent me and opened a new sketch on the Right plane. I sketched a couple of circles the same diameter as the gears, and a couple of tangent lines between them, then trimmed the circles and offset the sketch a certain distance, making the base construction, just like you see in this image.  Notice that this is not an assembly  sketch; it is actually inside a new part that was created in the context of the assembly.

El primer paso era crear la trayectoria que seguirían los eslabones. Para esto comencé con el ensamblaje que me envió mi lector y dibujé un croquiz en su plano de Vista Lateral. Ahí dibujé un par de círculos del mismo diámetro que los engranes y centrados en los engranes, y un par de líneas tangentes a estos círculos. Después de recortar los círculos y utilizar Offset terminé con un croquis como el que ven aquí. Noten que este croquis se encuentra dentro de una pieza nueva que ha sido creada en el contexto del ensamblaje.

Using this sketch, I extruded a surface. The width doesn’t really matter, since it’s merely an auxiliary surface.

Utilizando este croquis, extruí una superficie. El ancho de la superficie no importa, ya que es meramente auxiliar.

And now comes the tedious part: adding and matting all the links. Each link in the model my reader sent me had three parts that needed to be mated to each other using standard concentric and coincident mates.

Y ahora comienza la parte tediosa en la que se habrá de añadir los eslabones y las relaciones de posición para cada uno dentro del ensamblaje.  Cada eslabón en el modelo hecho por mi lector consta de tres piezas que tendrán que unirse entre si para formar la cadena usando relaciones de posición concéntricas y coincidentes standard.

Then, the cam mate was added between each link and the path.  To add a cam mate, simply click on Mate and then click on Mechanical Mates. Select Cam from the list of available mechanical mates. In the first field under Mate Selections, select all four surfaces that make up the path. You can easily select all four by right clicking on one of them and then selecting Select Tangency from the fly out menu. For the follower, select the cylindrical face of the link. Apply a cam mate for each one of these cylindrical faces in each and every link in the assembly. I told you it was tedious!

 A continuación, la relación de posición Cam (leva) se añade entre cada eslabón y la superficie que sirve de trayectoria. Para añadir la relación Cam simplemente selecciónala de entre la lista de relaciones de posición mecánicas disponibles.  En la primera casilla, se habrá de seleccionar las cuatro caras que conforman la trayectoria. Para el seguidor, selecciona una de las dos caras cilíndricas del eslabón. Para asegurar que el movimiento sea como deseamos, la relación de posición se habrá de añadir para todas y cada una de estas caras cilíndricas en todos y cada uno de  los eslabones en el ensamblaje. ¡Les advertí que esta parte era tediosa!

Since I didn’t have much time in my hands (or patience), I only added  enough links to see if the animation would work. I also added a coincident mate between one of the links and a planar face on the side one of the gears, to keep the chain from sliding to the sides when dragged. With these mates in place, the cylindrical faces of the links will always be tangent to the path and now every time we drag one of the links, they’ll all move along the path, like cars on a roller coaster ride.

Como no contaba con mucho tiempo (o paciencia), añadí únicamente los suficientes eslabones que me permitieran comprobar que la animación funcionaría de esta manera. Además  de las ya mencionadas, añadí también una relación de posición coincidente entre uno de los eslabones en la cadena y una cara plana del costado de uno de los engranes, simplemente para evitar que la cadena se deslizara de lado a lado.  Con estas relaciones de posición, las caras cilíndricas de los eslabones se mantendrán siempre tangentes a las superficies que conforman la trayectoria y cada vez que arrastremos un eslabón, éste y el resto de la cadena junto con él se desplazarán a lo largo de la trayectoria, como carritos en una montaña rusa.

Next step in the animation is to somehow make the gears drive the movement of the chain… or at least fool the eye into believing they are actually driving the movement.  Why am I saying this? Well, because although in real life a gear would drive the chain by coming in contact with the links and pushing them,  using contacts in Basic Motion is completely out of the question. It  just won’t work with the mechanical mates we just applied here. In order to use contacts in Basic Motion to have the gears actually drive the links we would have to suppress all the cam mates and use exclusively standard mates. I didn’t try this route, to be honest, because I didn’t add all the links to the chain. If any of you goes this particular route and finds it a great success, please, come back and tell me all about it.  

El siguiente paso en la animación era lograr que de alguna manera los engranes movieran a la cadena… o al menos, engañar a la vista y hacer parecer que la mueven. ¿Por qué digo esto? Bueno, porque a pesar que en la vida real el contacto físico entre los dientes del engrane y los eslabones es lo que provoca el moviento de la cadena, en el gestor de animación de SolidWorks no es posible usar contactos y relaciones de posición mecánicas como Cam en una misma animación. La animación simplemente no funciona. Si fueramos a usar contactos en el modo de movimiento básico (Basic Motion) para hacer que los dientes del engrane empujen a los eslabones, tendríamos que suprimir todas las relaciones de posición Cam que añadimos anteriormente y utilizar únicamente relaciones de posición de tipo estandar. Para serles sincera, no intenté hacerlo de esa forma, pues como dije anteriormente no añadí todos los eslabones a la cadena y este método requeriría de la cadena completa para comprobar si funciona o no. Si alguno de ustedes lo intenta utilizando contactos y le funciona, por favor regresen y cuéntenme como lo hicieron. Igual y cuando tenga un poco más de tiempo lo intento de esa manera.

So, back to Animation mode… Using other mates to try to relate the position of the links to the gears won’t be of much help, either. My reader had used a tangent mate between a cylindrical face of the link and one of the faces of the tooth adjacent to it to assure they remained adjacent to each other as the gear turned. This kind of works… sort of… at least for a short while. The chain does move as the gear rotates, but the mate cannot be satisfied all throughout the path the link most follow, so at some point it will actually prevent the assembly from moving any further and the animation fails.  So, we won’t add any other mates; instead, we’ll simply try to coordinate the positions of the chain and gears at several points throughout the animation, so it seems like the gears are actually driving the chain.

Por el momento, de regreso al modo de Animación… Mi lector intentó usar una relación tangencial entre la cara cilíndrica del eslabón y una cara adyacente en el diente del engrane para asegurarse que ambos componentes se desplazaran juntos a medida que el engrane giraba. Esto funciona… más o menos… por un periodo muy corto. Al principio, el engrane parece empujar el eslabón y la cadena se mueve con él, pero en poco tiempo el moviento se interrumpe por completo, tan pronto como la relación de posición tangencial deja de satisfacerse y la animación falla. Es por esto que no añadiremos ninguna relación de posición para tratar de ayudarnos y simplemente trataremos de coordinar la posición de la cadena y los engranes en varios puntos distintos a lo largo de la animación, para que parezca que los engranes son los que mueven la cadena.

First of all, we need to begin with a good position. As you can see in the image, I tried to position the link in between two of the teeth in such a way that it didn’t appear like there was some interference between them.

Primero que nada, se tiene que comenzar con una buena posición. Como ven en la imagen, traté de ubicar el eslabón entre dos de los dientes de forma que no diera la impresión de que había interferencia entre ellos.

Now, we can create a new motion study and chose Animation mode. With Autokey depressed, move the time bar to a new position in the timeline and drag the first link along the path. You can try to position it between another couple of teeth, just like earlier, and count how many spaces there are between your original position and the new position. This is just to help yourself along the process.  I moved mine two spaces counterclockwise. A new key point is created in the timeline.

 Una vez que se tiene una buena posición inicial para el modelo, podemos proceder a crear un nuevo estudio de movimiento, utilizando el modo de Animación. Con el Autokey presionado, arrastra la barra vertical de tiempo a una nueva posición en la línea de tiempo (dos segundos en este caso) y luego arrastra el primer eslabón de la cadena a una nueva posición relativa a la que estaba antes. Para ayudarte en este proceso, puedes tratar de ubicar el eslabón entre un par de dientes y contar el numero de espacios entre la primera posición y la nueva posición. Yo moví mi eslabón un par de espacios en el sentido contrario a las manecillas del reloj. En la línea de tiempo, los cambios son registrados.

Now drag the gear’s tooth that used to be next to that link counterclockwise two spaces to  it’s new location, right next to the link you just dragged. Again, try to position it in such a way that it doesn’t look like there’s interference between the tooth and the link. Click calculate and observe the animation. If you see like the gear appears to be going through the links despite your best efforts to position them correctly, you probably need to adjust the number of frames. The bigger the number of frames, the better your animation will look in this case, although calculations will probably take a little longer.

Ahora, arrastra dos espacios el diente del engrane que solía estar junto al eslabón que se desplazó anteriormente y colócalo en su nueva posición, en la misma posición relativa que tendría junto al eslabón si ambos se hubieran desplazado juntos. Igual que se hizo al principio, trata de que no paresca haber interferencia entre ambos componentes.  Haz click en Calcular. Si a pesar de tus esfuerzos por colocar los componentes apropiadamente, en la animación parece como que un componente atraviesa al otro, talvez lo que necesitas ajustar es el numero de imágenes por segundo (frames) de la animación. Entre mayor sea este número, mejor lucirá la animación, pero el cálculo tomará más tiempo.

For some reason that I still don’t understand completely, you can’t simply continue dragging the chain and adding keys automatically after this point. It doesn’t seem to work correctly. At least, it didn’t seem to work for me. I mean, a key point was created, but the chain didn’t update its position in the animation. Weird…  So… Instead of that…  Undepress  Autokey, drag the time bar to the next position in the timeline, select the  component to move from the tree on your left   and click on Add/Update Key to create a new keypoint for this component. Then drag the component (and the chain with it) conterclockwise a couple of spaces along the path like you did before.

Por alguna razón que aún no acabo de entender, no me fue posible simplemente arrastrar el eslabón y crear un nuevo punto en la animación como hice anteriormente. El punto aparecía en la línea de tiempo, pero la posición de la cadena en la pantalla no cambiaba en lo absoluto. Para remediar esto y continuar con la animación, haz lo siguiente: Desactiva Autokey, arrastra la barra vertical a una nueva posición en la línea de tiempo (cuatro segundos), selecciona el componente a arrastrar en la lista de componentes del lado izquierdo and haz click en Add/Update Key para añadir un nuevo punto en la línea de tiempo de la  animación para este componente, después de esto, arrastra el componente (y el resto de la cadena junto con él)  dos espacios en la dirección contraria a las manecillas del reloj como se hizo antes.

Depress AutoKey again (It’s important that you do this before continuing) and drag the gear to its new position, just like you did previously. A new keypoint will be created for the gear. Click calculate.

Activa AutoKey nuevamente (Es importante que hagas esto antes de continuar) y arrastra el engrane dos espacios a su nueva posición, como se hizo anteriormente. Un nuevo punto en la línea de tiempo de la animación se creará automáticamente para el engrane. Haz click en calcular.

Continue doing this until you manage  to complete at least one time all around the path (this is assuming you have all the links in the chain). This is time consuming, I know, but if it’s done with care it can actually produce a very nice animation.  Ah, and don’t forget to hide the auxiliary surface so it doesn’t show up  in the animation by right clicking on it in the tree and selecting Hide. If you wish, you can add a belt/chain (Insert, Assembly Features, Belt/Chain) between both gears to make the other rotate at the same time and the same angle when you rotate the first one.

Continúa haciendo lo mismo que se hizo en los dos últimos pasos hasta que se haya logrado al menos una vuelta completa al rededor de toda la trayectoria. Este proceso se lleva tiempo y es un poco tedioso, es verdad, pero pienso que si se hace con cuidado puede producir buenos resultados. Ah, y no se te olvide esconder la superficie que se usó como trayectoria para que no aparesca en la animación. También puedes añadir una relación de cadena o banda entre ambos engranes, para que se muevan la misma distancia angular y al mismo tiempo.

This is a video of the small bit of animation I made. Of course, I don’t have the whole chain here, but it’s just for you to see what I’ve been talking about in this post. Seriously, if one of you comes out with a simpler and easier, fool-proof way to do this IN SOLIDWORKS, let me know and I may even treat you to a SolidWorks baseball cap like those they are selling at their online store.

Este es un pequeño video del pedacito de animación que hice. Por supuesto, aquí no tengo la cadena completa, pero quería que lo vieran para que me entiendan mejor de lo que he estado hablando en este blog. En serio, si alguno de ustedes encuentra una manera más sencilla, rápida y a prueba de errores de hacer esta animación EN SOLIDWORKS, por favor, cuéntenme y muéstrenme pruebas de cómo le hicieron y hasta puede que les dispare una gorra de SolidWorks de las que tienen de venta en su tienda de artículos promocionales.

I’ve never really been a car enthusiast. I mean, I like race cars and I sure enjoy the looks of a few models, like this particular one that was parked at some sort of car expo near the amusement park a few weeks ago. Isn’t it a real beauty? I actually like this one better than its younger cousins that were also on display that day.

 Anyway, I like to look at cars and I like to drive them, but I’m certainly not the kind that can remember makes and models, let alone identify all the different pieces that form part of a vehicle.  Last night, however, and out of sheer curiosity after reading a post from the SolidWorks Discussion Forums where someone was asking for examples on how to use the universal joint mate and someone else suggested looking at a drive shaft, I found myself searching the internet, trying to find pictures and information about cars and transmissions and what not. I eventually found some really nice assembly pictures for a 280Z, and my husband,  who  by then had grown curious about my sudden interest for cars, was more than glad to explain to me how each of those parts was supposed to work.   I never thought I would say this, but it was actually very interesting and even kind of fun.  Or maybe he’s just a good teacher, who knows?

This is one of the images I found for the drive shaft.

After taking a long look at it, I went back to SolidWorks to try to find some information on how to use the universal joint mate, but I couldn’t find much in the help. I guess it’s because it’s not really such a complicated mate?  So, I put together my own universal joint assembly to experiment.  The universal joint, also known as Hooke’s coupling, is used to connect two intersecting shafts, and apparently has its widest use in the automotive industry.  A simple model of the Hooke-type universal joint is shown in the following image. The small shaft could be the driver, the long one could be the follower and the third link is a cross piece that connects the two yokes. 

 As the driver rotates, it transfers this rotation to the second shaft.  In SolidWorks, the universal joint mate is useful for those cases when you need to transfer rotational motion around corners or, like in the case of the driver shaft of a car, between two connected shafts that are allowed to bend at the connection point.  

I actually came up with two versions of the same assembly, one with the third link connecting the two shafts, and one where that link is missing. The one without the link uses the universal joint mate, while the other one relies on the link to transfer rotation between the shafts. The results of using one method or the other were pretty much the same.

So, to add a universal joint mate between two components, simply  select  it from the mechanical mates group, and then, under Mate Selections,  select the two components you wish to mate together (in my case the two yokes)  and, as an option, define the joint point.  The joint point (in purple in the image) represents the connection point between the two components. In this case is the point where the axis of one shaft intersects the axis of the other.  Since I didn’t have a physical component connecting both shafts, I actually sketched a point to serve as joint point and located it where the center of the missing link would be.  Just as in the case of other mechanical mates, such as gear mate and rack and pinion mate, this mate will work even when the components don’t actually touch each other or have any other component to come in touch with both and connect them, but you’ll need to add other mates to the mix in order to control the position of the elements in the screen and with respect to each other. In my case I mated the axis of each shaft coincident with a couple of reference axes that intersect each other at the joint point.

I added a rotary motor to the driver shaft and then ran the motion study.  I’m sorry I didn’t actually make a video of this one, but it’s only ten seconds worth of animation, so I didn’t see the reason for it. This is an animated gif; if you double click on it you’ll be able to see the movement of the universal joint.

I was actually planning on posting about friction coefficients and the way it all works using an example of a simulation of these tong grabs, but before I do that, I thought I should share with you about a little problem I ran into while trying to use a special option available for the hinge mate and a way to work around it.

OK, first of all, let me tell you a bit about what these tong grabs do. Tong grabs or friction tongs are very clever contraptions that are often used to lift heavy, bulky loads.  The principle behind them is very simple:  as you pull them up, the tongs close on the sides of the object you wish to lift, if the friction coefficient between the object and the surface of the tongs that comes in contact with it (usually known as pads) is big enough, then the tongs will be able to lift the object.  Mine is a very simplified model, just for illustration purposes. There are several different kinds of tong grabs available, depending on the kind of load you wish to lift. I found some inspiration in the ones available from Bushman Equipment.

If you check the ones available from that site or some other, you’ll see that some of them have adjustable pads that come in touch with the load and that rotate a few degrees in order to accommodate wider or narrower loads. These pads are also often furnished with rubber, belting, or other materials to increase the friction coefficient as needed. I wanted to add some very simple rotating pads to my model, but I also wanted to limit their rotation to only a few degrees, to ensure they would not rotate to the opposite side or hang flat as the tongs were closing on the load.  For this purpose, it occurred to me that I could use a special kind of mate known as the Hinge Mate, and take advantage of the option “specify angle limit” available for this particular kind of mate.

The Hinge Mate is a mechanical mate that comes in pretty handy when running a motion study, since it’s usually recommended to add the kind of mates that will allow the model to behave as close to how it would do in real life as possible. In other words, if it behaves like a hinge, use a hinge mate. Think of how you usually mate the hinges of a door, for instance, you usually need two mates: concentric and coincident. The hinge mate combines those two mates in one and even offers the option of specifying a limit for the angle of rotation between the two components that form the “hinge”.

In the image, the hinge mate is being added between the grabs and the pad. The concentric selections are the cylindrical faces of the holes in the pad and the grabs. I’m not using any fasteners in this model, but if I was, this would be the hole for a bolt, pin or screw. The coincident selections are two faces that come in touch, shown in purple.

The option “specify angle limits” is being used here to limit the angle of rotation between the surfaces highlighted in pink.  The first value (50 degrees) is the current angle between the two surfaces, the second value is the maximum value that can ever be between those two surfaces and the third value is the minimum angle. This means that the pad will be able to rotate anywhere between the minimum and maximum angle as needed, depending on the width of the load.

 This is really cool, only problem was that when I tried it with my pads and ran the motion analysis, the “specify angle limit” option didn’t work at all. So, I asked the folks from SolidWorks if it was that this particular option wasn’t supported in SolidWorks Motion and they said to me that it is supposed to be supported, that this is not a bug, but a known issue still present in SolidWorks 2009 SP4.0, and they are working to fix it as I write this.  It may be fixed in a future service pack or release, but in the meantime, there is a way around it, and Mr. Matthew Derov, training specialist at DS SolidWorks, was really kind to explain to me how.

Here I share what he told me with you, in case you run into this same issue:

“The “Specify angle limits” option for hinge mates should be supported when using motion analysis.  This is actually a known issue and our developers are working on getting it fixed.  In the meantime, a work around for this issue does exist.  To specify an angle limit for your mate, de-select the “Specify angle limits” option in the hinge mate and set up a separate advanced “Angle” mate with a maximum and minimum angle.  I have attached a simple model for you to have a look at how I set it up (Motion Study 1). “

This is a screen shot of the model he attached. You can see that there are two mates between these parts: the hinge mate and the limit angle mate.

In this image you can appreciate the way he set up the hinge mate for the assembly.

 

“Please also note that a separate issue exists with the angle mate and motion analysis.  If your parts begin in perfect alignment (angle set to 0 degrees in attached model) there exists 2 separate solutions to the problem and the solver will not handle this properly.  Therefore, you must offset the starting angle slightly to define the angle direction.  This is also a known issue being worked on by our motion developers.  If you specify a slight offset (i.e. 1 deg) as done in my example, the solver will compute the solution correctly.”

This is a screen shot of the way he set up the limit angle mate in his example. Notice the small one degree offset that he’s talking about.  

 

The study he set up in Motion Analysis included only the force of gravity acting over the assembly, as you can see in the image.

 

One of the parts is fixed, while the other one can rotate within the range specified in the limit angle mate.  This part rotates by the effect of gravity, but stops when it reaches the value of the angle he specified earlier as the maximum limit.

 

Hope you find this information useful!