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Archive for May, 2009

As I had mentioned previously, and also in a comment to my last post, I’m  currently teaching myself SolidWorks Motion, with the aid of the official  2009 training manual. I’m really enjoying the exercises and examples provided in the book, and the way everything always turns out as predicted in the lesson.  My problem began, however, when I tried to use Basic Motion to run some examples of my own. 

For those of you that are not familiar with SolidWorks Motion, let me explain briefly that there are three different modes that can be chosen from the Motion Manager:

·         Animation, MotionManager animation. Used for basic SolidWorks Animations

·         Basic Motion: MotionManager advanced animation. Used for more advanced SolidWorks Animations where more realism is required. This solver accounts for some aspects of dynamics such as inertia, contacts etc., so the animation is realistic.

·         Motion Analysis: This is SolidWorks Motion solver, rigid body dynamics solver that provides accurate numerical results (displacement, velocities, forces, etc.).

It is clear for me now that these are two different products: SolidWorks Animation, if you want to call it that way, and SolidWorks Motion, although both accessible from the same MotionManager. Anyway…  My problem seems to be then with the animation part of it, more particularly with Basic Motion.

The problem became evident when I tried to simulate the movement of my arbor press assembly. I wanted to show the gear rotating and transmitting that movement to the rack. For this purpose, I used a rotary motor on the gear and the rack and pinion mate took care of the rest. My animation would’ve shown the rack going down until, like in the real thing, the rack pad met with the table and the movement had to stop.  Animation mode couldn’t do this for me because in this mode the movement of the components with respect to each other is constrained basically only by the mates you add to the assembly, and it doesn’t simulate physical contact between components. In other words, if two components come in touch, they can go right past through each other and the collision is never detected.

I decided to use Basic Motion, which is the advanced animation mode because it simulates physical contact between components in the assembly. Of course, you have to tell SolidWorks  which components are to have contact between them, but once you add a contact the simulation is supposed to acknowledge it and produce results accordingly. In my case, adding a 3D contact between the rack pad and the table should’ve been enough to stop the movement when the two components came in touch and prevent the rack from going through the table as it did before in Animation mode. Only it didn’t work.  The contact I had added between the table and the rack pad was not acknowledged and the rack again went through the table, just like it did in Animation Mode. The funny thing is that I created a second motion study, again in Basic Motion mode, and I tried using a linear motor on the rack, instead, and this time the contact between the table and the rack pad was acknowledged, although with a bit of penetration.

I have been searching for answers on this and trying different things, just hoping to figure out what it is that I’m doing wrong. I tried adding gravity to the simulation, again in Basic Motion, and I observed something unexpected:  the contact between the table and the rack pad was suddenly acknowledged, and the motion stopped when the two components came in touch with each other and without any penetration at all.  However, the effect of the rotary motor in the simulation was absolutely null. I know this because I changed the direction of rotation of the motor, to make it now move the rack upwards, but the rack continued to go down by the effect of gravity, as if the motor wasn’t even there.  A linear motor on the rack, however, did move the rack up in this case.

Puzzled by all this, I went to the SolidWorks forums and found that some other users had seen similar results when using motors and contacts in Basic Motion. One of them suggested the possibility of a bug. It kind of felt nice to know that I wasn’t the only one seeing this; but still, it gives me no answers and no solution for the problem. I was more and more confused by the minute… I mean 3D contacts and rotary motors sure worked for the examples provided in the book, why wouldn’t they work for my own examples? What was I doing wrong?  It was then that I ran into a particular exercise in the training manual that included a rack and pinion, very similar to mine. The example is a catapult that uses a rotary motor to move a group of gears and a rack and pinion mate to transmit the movement of the gears to a rack that pushes a small trigger attached to its end. This trigger must come in contact and push a second trigger which is part of a projectile holder mechanism.  For this to happen, a 3D contact must be added between the two triggers.  While this example works beautifully in Motion Analysis mode (remember this is the SolidWorks Motion solver), I discovered that, just like mine, it won’t work in Basic Motion.  Basically, both triggers will simply go past through each other, never acknowledging contact between them, never detecting a collision of any kind, and that kind of ruins the whole animation, don’t you agree?

I took a look again at the exercises from the training manual where rotary motors and contacts had been used successfully in Basic Motion mode and noticed that they didn’t involve the use of gear mates or rack and pinion mates at all. I ran a quick and simple example of my own using the two components in the following image. The idea was to use a rotary motor to rotate one of the two components and add a contact between them, so the movement of the first component would cause the other one to move once they came in touch with each other. This worked fine in Basic Motion mode, and is basically what the examples of the training manual were like.

Next, I added two more components just at the right distance from the first two, and contacts between them two and between the two sets of outer rotors, and again, the simulation ran perfectly fine in Basic Motion, and pretty soon I had the first set transmitting its movement to the second set, the motor worked, the contacts worked. 

The problem came when I removed the contacts between the two outer rotors and added a gear mate between them instead. When I ran the animation in Basic Motion mode, the contacts between the first set of rotors are ignored and the first rotor can’t even seem to be able to complete one full rotation; it remains stuck half-way through it. Other unexpected results are also observed.  Needless to say that the example runs perfectly fine if I change to Motion Analysis, but as I was told, that’s  the Motion Solver, completely different from Basic Motion, which is simply an advanced animation mode.

So, I guess this means that gear mate and rack and pinion mate aren’t really supported in Basic Motion mode in 2009? Is this a bug or was it always supposed to be this way? In case it is supposed to be this way, what other mates aren’t supported? I’ve searched for information about unsupported mates, but haven’t found anything about these two mechanical mates so far. IF it is a bug (bad bugs happen to good software too), I just hope it gets fixed soon. I really enjoy using SolidWorks, and it’s a little discouraging when it doesn’t quite perform as expected.  Anyone has any ideas on this or has observed this before? Anyone has found a fix for it?

 

My son made me promise this was really a model of lip balm… less girly I guess, if you’re willing to overlook the flowers on the decal, that is. Sorry, I couldn’t resist! Not that I usually wear lipstick, err, lip balm, but when stressed out to the max and whenever tossing a 12 lb ball at a group of unsuspecting pins won’t make me feel any better,   I often find solace in regular things and activities that have long been considered exclusively feminine. That’s the good thing about being female! Yep, sometimes even a dab of lipstick can do the trick! Ah, but this one here is no ordinary lipstick! Putting this SolidWorks model together was possible thanks to the use of two special mates: the screw mate and the width mate.

OK, so this is the lipstick assembly. It is made out of three different parts: One I’ve called the lipstick bottom, which is the part at the bottom of the tube, the one that you usually twist in order to get the color to come out. This part is cylindrical and has a couple of vertical guides (slots) on each side.

Another part of this assembly is the one I called lipstick top. This cylindrical part has a couple of helical guides on the inside, and the cylindrical part previously described (lipstick bottom) fits inside of this one.  The helical guides were created using a sweep cut of a rectangular profile following a helical path. The helical path describes only one revolution as it travels from bottom to top of the part. Notice in this case, the cylinder has a height of 2 inches and that’s precisely the pitch of the helix. The second guide is created by patterning the first cut.

And finally, the third part is what I called the lipstick content. This is the part that has the creamy color. This is also a cylindrical part with a couple of pegs on the sides. These pegs will have to follow both the helical and vertical guides on the other two parts for the lipstick to work as such and for the color to travel up and down the tube as the bottom part is twisted. The idea is simple, as the bottom twists, the vertical guides push on the pegs and force the content part to rotate; as the content part rotates, the pegs follow the helical path on the lipstick top part (which remains immobile), thus translating the whole content part up or down, depending on the direction of twist.

How to make sure the pegs follow the guides? Well, this is where the mates come in handy! First, the width mate. The width mate is a very simple, yet extremely useful, mate among the advanced mates available in SolidWorks. What it does is to center the peg within the width of the vertical slot.  In order to use this kind of mate you will always need to provide references for the width (it could be a groove or some cavity and you’ll need to provide two parallel planar faces or two non-parallel planar faces) and for the tab (two parallel planar faces, two non-parallel planar faces like in a wedge, or a cylindrical face or axis). In my case, my tab reference is the cylindrical face of the peg and my width references are the two long planar faces of the vertical slot.

And now for the screw mate. This is one of the mechanical mates available in SolidWorks and what it does is to constrain the movement of two components to be just like in a real screw, concentric and with a pitch relationship between the rotation of one component and the translation of the other. What it means is that by applying this kind of mate to the lipstick content  part (the one with the pegs) and lipstick top part (the one with the helical guides), the rotation of one of these parts will cause the other part to translate along the axis.  As you can see in the image, I selected the axis of each part as the entities to mate and set a distance/revolution value of two inches, because, if you remember, that’s precisely the pitch of the helical path that was used in creating the guides. This means that, as the lipstick bottom part rotates the lipstick content part with travel 2 inches up or down per each revolution. This will make it look like the peg is actually following the helical guide.   The option to reverse the movement simply changes the direction of movement, clockwise or counter clockwise, as needed.  

After applying a few other mates to the assembly, such as mates to prevent movement of the lipstick top part (the one with the helical guides), we have a model of a lipstick that works pretty much like the real thing and we can see it move simply by dragging the components or by using SolidWorks Animation.

This is a short video I put together on using SolidWorks Motion to simulate the movement of an arbor press. This is really my first try on animation, I mean, besides the examples and exercises on books and tutorials. I’m currently learning at my own pace using the SolidWorks Motion training manual. There’s also a book called The Step by Step Self-Study Guide to SolidWorks MotionManager.

I was planning on having this video ready last week, but I caught my son’s pneumonia and my plans had to change… Well, here it is and I hope it helps someone out there that is also trying to learn about SolidWorks Motion. Just click on the image below to go to the video.

You can also watch and download this video at Viddler.

And by the way, happy Mother’s Day to all the moms out there! I’m having a wonderful day myself, thanks to a sweet husband and a couple of kids that woke me up at the crack of dawn just to shower me with cards and little presents!

 

Well this turned out to be a two part post, instead of one. It all started with me venturing into SolidWorks MotionManager, which is used to create little animations of assemblies as they are exploded and/or collapsed, rotated, dragged around, or just made to have their components move and interact with each other in the way they would do in real life. I’m working on a little video about it, using this assembly of an arbor press.

That’s the subject of my next post, but for now I wanted to tell you about the spur gear and the rack that form part of this assembly, if only because this is something I hadn’t tried before, because it required a bit of extra effort, and because displaying this information here might benefit someone else that is trying to do the same.

First of all, let me tell you where that spur gear and rack came from. I would love to say that I modeled them myself, but that would be a lie. No, I used some handy Toolbox parts, instead. If you’ve never used the Toolbox, maybe you should give it a try. Granted, you can’t really use the models of gears generated this way for manufacturing purposes, but they are at the very least a decent representation for when you need to simulate movement, like in the case of my arbor press assembly. So, if you have Toolbox with your seat of SolidWorks, go to the folder marked as Power Transmission, select Gears, right click on Spur Gear and then select Create Part from the menu.

A new part will open and you’ll see a model of a spur gear on the graphics area. Don’t despair if that’s not the spur gear you want, just wait for the property manager that will open to the left.

In this property manager, you can enter information about the gear you wish to generate, such as:

·         Diametral Pitch, which is the ratio equal to the number of teeth on a gear per inch of pitch diameter. The Pitch Diameter is the diameter of an imaginary pitch circle on which a gear tooth is designed. Pitch circles of two spur gears are supposed to be tangent for the gears to work. In the case of the spur gear and rack, the gear’s pitch circle must be tangent to the rack’s pitch line, which is the construction line in the middle of the tooth cut.

·         Number of teeth

·         Pressure Angle, which is the angle of direction of pressure between contacting teeth. It determines the size of the base circle and the shape of the involute teeth. It is common for the pressure angle to be 20 or 14 1/2 degrees.

·         Face Width, that’s the width of your gear.

·         Hub style and shaft diameter

·         Number of teeth to show

Once you enter this information, SolidWorks takes care of the rest and generates a model of your gear. You can then save it with a different name and add other features to it, like I did. Like I said before, this is not the proper way to design a gear, but only a way to obtain a decent representation of it.

Generating the rack involves a very similar process. From the same Gears folder, right click on Rack (spur rectangular) and select Create Part. You’ll see a similar property manager open to the left of the graphics area.

Once again, you are asked to provide values for the Diametral Pitch, Pressure Angle and Face Width. Diametral Pitch and Pressure Angle values should be the same ones you provided for the Spur Gear. You will also be asked to provide a value for the Pitch Height; that’s the distance measured from the pitch line to the bottom face of the rack. Once you have all your values ready, SolidWorks will generate a model of the rack for you. This rack can be used with the spur gear generated previously to simulate rack and pinion motion, with the use of a special mechanical mate, called, umm, the rack and pinion mate.

The rack and pinion mate is used for relating power transmission involving rotation and translation.  This can apply to a spur gear and a rack, or even to a wheel rolling on a surface. In this image you can see the case of a “wheel” and surface. In this case the wheel is resting on the surface of a little track and, besides other mates to prevent the wheel and track from wandering all over the graphics area, I applied a tangent mate between the circular surface of the wheel and the top surface of the track, just to make sure the wheel remains in touch with it as it rotates. Then, from the mechanical mates, I applied a RackPinion mate to the wheel and the track. For the rack definition, I chose an edge at the bottom of the flat track, and for Pinion/Gear definition, I used the edge of the wheel, as you can see in the image.  SolidWorks calculates what would be the pinion pitch diameter, which in this case is simply the diameter of the wheel. As a result of applying this mate, every time I rotate the wheel to the right, the track will slide to the left and vice versa. Notice, however, that in general, the use of this mate doesn’t even require that the two components come in contact with each other. For instance, if instead of applying the tangent mate between the surfaces I had applied a distance mate, leaving a considerable gap between them, the track would still slide to the left whenever the wheel rotates to the right. In the case of gears and racks, it means that simply applying this mate won’t provide the look of accurate motion; you have to do a couple other things to make sure it looks realistic.

First of all, if you look among the features listed for the spur gear, you’ll find a cut extrude feature named ToothCut, if you expand it, you’ll see a sketch by the name of TooCutSke; that’s the sketch of the teeth and pitch circle, so make sure it’s showing in the assembly (right click on it and select show). In the case of the rack, the sketch you are looking for is under ToothCutSim, by the name TooCutSkeSim. Make sure this sketch is also showing.

Before applying the RackPinion mate, locate the pitch circle in the gear’s sketch, as well as the pitch line in the rack’s sketch, and apply a distance mate between the center of the spur gear and the pitch line of the rack. The distance value must be the radius of the pitch circle. This is to make sure you have good tangency between both components. As I said before, with the RackPinion mate alone, you could have the spur gear and rack 20 feet away from each other, or vice versa, completely interfering with each other, and they would still move about, but that wouldn’t look very realistic, now would it? Another thing you need to do before applying the RackPinion mate is make sure the teeth or the spur gear and rack are meshing properly, that is that they are not interfering with each other. Adjust them if they are.

Now you are ready to apply the RackPinion mate. Under Rack definition, select any linear edge of the rack in the direction of travel. I used the lower edge of my rack for that purpose. In the Pinion/Gear definition, select the gear’s pitch circle. The property manager updates immediately with the value of the pinion pitch diameter, which is the same diameter of the spur gear’s pitch circle. Click OK and test the mate. If the rack is moving in the wrong direction, then edit the mate (rick click on it and select Edit) and mark or clear the Reverse option, then test again.

Not bad, huh? And you’ll see it in action in my next post!