how to insert joints

[chris44]

hai everybody,

this is chris. i am a beginner to autodesk inventor. i am trying to simulate a model which converts circular motion to elliptical motion (just like elliptical exercise machine...same concept) but i am stuck at simulation. first of all i am not sure how to insert joints

can someone plzz help me

i am also attaching the file. the shaft is connected to the circular disc. force is applied at the shaft. as the disc rotates, the rod connected to the disc should move in elliptical motion while sliding on the base. can someone help me how to simulate the model


many thanks,

chris

[shift1313]

hey chris. are you simulating this in Studio or in Dynamic simulation. Im guessing by the terminology JOINT that you are in dynamic simulation but i want to be sure.

In the assembly mode if everything is modeled properly you can right click on your part names in the model tree and select ContactSet. This will allow you to manually move your parts and see their interaction. You can also drive angular constraints to analyze the motion.

Simple mates like concentric can be brought into Dynamic simulation. You will have to make special note of the grounded folder. anything in there will be "fixed" meaning it has not be accurately defined for motion.

When creating joints there is a rather good animation in the selection box that helps you pic your items in order(next to the drop down box is a button to display joint table). I would suggest you open up dynamic simulation help file. It will walk you though the basic concepts of joints and how/when to use them.

Just listening to the problem id say you need a standard revolution joint. it should be the one with what looks like a door hinge in the animation. For the "foot" of the tread it will be a sliding cylinder on a plane in the sliding joints category.

A lot of this really depends on how your model is setup. if some joints are sliding or rolling(bearings/wheels) and so on. There is a post limit before you can post links and i think attach files. 5 posts maybe.

[chris44]

thanks for the quick reply shift, i really appreciate it.

i am simulating my model in dynamic simulation. i hope in the assembly model i fixed each and every part correctly ( i just did the mate constraint thing for all the 3 parts).

i am attaching the zip file. if you have time can you please look at it.
the shaft is connected to the circular disc on the back side (iam thinking to apply the force on the shaft, to make the circular disc to rotate, i dont know whether this works or not).

thanks a lot,

[shift1313]

hey chris. I dont have inventor 2010 at work so i cant open the file until i get home. Are all the parts included as well as the assembly file? If not you will need to attach each .ipt file that is referenced in the .iam file(that you are concered with). ill take a look at it this evening for you.

[chris44]

hai shift,

yes, i attached the assembly file....and the part files associated with it. i guess, it should be easy to you....bcoz it is not a complex one....but since i just turned to inventor...iam goin nuts to simulate this thing.

by the way i have gone through the simulation tutorials...atleast it gave me an idea....(thanks for that). i really appreciate it, if you take some time to look at the model and give me some suggestion how to simulate it.

many thanks,

chris

[shift1313]

Alright chris, i have an older version of inventor at work so i drew something real quick for you. I drew 4 parts. I have something that is the pivot point for both the "wheel" and for the upper link(which would be the handle). I have 4 constraints added to the assembly. All of them are "insert" constraints. This insert constraint will allow the parts to mate but still allow rotation. You can apply these mates to your parts and rotate them using the mouse in the assembly. In this case we are talking about simple mates, no real mechanical mates like interference or path driven stuff.

So - insert constraint at the wheel center, the first link to the wheel, the links together, then the second link back to the base. In my case the base is just a blue piece that has two "studs" on it for the wheel and link to pivot.

When you start the Dynamic simulation you will have a tree on the left side just like the assembly environment but this will have all your components, loads, joints etc. When you first start all components are grounded. This is because mates from the assembly arent automatically brought in. There is a Convernt Assembly Constraints button. This takes the constraints you already have and creates joints from them(if possible). This works fine for Insert Constraints.

It will ask you to select two components and it will analyze the joint between them and show you what its going to create(if you check the box). In this case you should end up with 4 spatial joints, 3 components listed under the Mobile Group heading and your base(Pin1 in my case) will still be grounded.(see image 2)

This should accurately(in this case) define the assembly. Now you just need to add force or torque. I added a small torque to the wheel. you need to watch your selection process on everything. It asks for a location and direction. i made a short .avi but i have to clear some space to host it.

[shift1313]

here is a zip file of the short video
http://filebox.vt.edu/users/maperez/eliptical.zip

[chris44]

thanks a lot shift, i really appreciate what u have done....tonight i am gonna work on this model...if i have any questions i will let u know...

once again thanks a lot,

chris

[shift1313]

Hey chris i took a look at your file this morning. one part didnt come in(a bolt) but thats fine, dont need it. Im assuming your "wheel" is rotating around the pin sticking out of the back of it and not the center right? The way the parts are oriented will make the leg loose contact with the track.

The first thing i had to do was change one of your constraints. The two threaded holes that were for part 6 and part 1. I deleted their constraint and added an Insert constraint only. It looks like you had an insert constraint with the bolt but since that component didnt load it was unresolved. After that I created a nother part named Base that I could have the wheel pivot on. Its important to have grounded components(like your track was) to ensure certain geometry cant change in the assembly. Without some sort of structure the components have too many degrees of freedom and will not behave how you want.

Just a note. Insert constraint not only locate two components concentrically but it will also mate with a certain offset. Part 6 had a mate, tangent and an insert. The mate constraint was not needed because the insert would take care of this. By selecting two circles(one on each part) you can model this without that bolt or any pins. This may be easier while you are trying to figure things out.


One extra note from the pics/info i posted before. Inventor 2010 automatically analyzes and creates the joints based off assembly constraints. The older version i was working in doesnt and i forgot about this until just now.

When you bring your assembly into Dynamic Simulation you will still need to create one joint which does not automatically get created. You will need a Sliding Joint - Cylinder on Plane. When you are creating this joint pay attention to the animation and selection process. First it asks you for a plane. Then an origin. If you look the origin is created but you can move it it you like. I selected the plane, then clicked on 2 to select the cylinder and then OK letting Inventor create my origin. The origins become extremely important but in this case the auto-created ones are good.
When you apply a torque to your wheel, select the outter edge of your wheel first, then select the outter face. The value i used was very small. .005. Since there is no resistance, springs, friction and so in there is not much force needed. You could simulate the weight of a person by adding a foce on the link down.

Hopefully i explained that enough to give you a start. Let me know if you have any questions.

[chris44]

hey shift....that was really helpful....if u dont mind can u please send me those files which u worked on inventor 2010

i really appreciate ur time...thanks a lot,

chris