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

[shift1313]

I didnt save them chris. From the drawing you sent, its really very little work. Ill re-open it and see what i can do. As a note i use educational versions so it will come with that watermark if you open it.

[shift1313]

sorry chris, the assembly file when i compress it is larger than the size limit here.

I can walk you through step by step if you need, but everything is outline in the above post. Im not sure if i mentioned it but I did add one other mate. The side of the roller to the side of the track.

[chris44]

hai shift,

that was really really helpful....now i simulated the model..its running good....as u said i applied a wheel pivot to circular disc (so that it just revolves around its axis). that was a simple elliptical machine mechanism...but i wasn't sure where to apply the joints...(i guess i wasn't that good at basics :unsure: ). without you helping me, i wouldn't have simulated it....thanks a million.

now i am going to design a complex elliptical machine ( its not that hard for u..:wink:). i am designing the model (the one on the zip file)....if i have any doubts or if i get stuck anywhere.....if u dont mind can i leave a message....?

once again thanks a lot,

chris

[shift1313]

We are always here to help chris. I am by no means an expert with this stuff and there are other users in here that can help as well(although the inventor forum doesnt see as much activity as some of the others). I dont mind at all for you to send me a message or email if you like, but you may get more out of it just posting here. With this stuff there are usually many ways to approach the problem. While the info/method I gave you may work, another user may have another approach that may work better.

Note on joints. When adding joints to your assemblies, a spatial joint is a catch all. It allows you to control each degree of freedom(6 of them). You will notice when placing the origin there are 3 axis, each with a different number of arrow heads. When dealing with two components, aligning the correct axis is important between the two. Say for instance you were creating a pneumatic cylinder and were trying to make the inner cylinder slide inside the body. Aligning the axis of both pieces and having only the degree of freedom along that axis will define this.

I suggest you start with some simple parts before you get too deep in your design:) Its very easy to get in over your head with this stuff. And have fun

[chris44]

hai shift,

this is chris...i hope u remember me.....i got a small problem.

as in my last post i attached a zip file of elliptical exercise machine...now iam simulating that machine using dynamic simulation and i got stuck with the simulation.

iam attaching the zip files...if u have some time can u please look on those things....

i encountered an error when iam doing the sliding joint to part 7 and part 11. it says the mechanism is over constrained by 1 degree(s). use repair redundancies command if the automatic joint creation is not active. then i tried fixing it....from the model tree where the error was by doing the surpress joint....but when this is done part 7 doesnt work as it suppose to work

and one more thing, the circular disc(part 13) is not rotating....(even though it has a rotational dof)

if u some free time...can u please give me some suggestions how to fix these things.....i really appreciate ur help...

i tried to attach the zip files....but the size was larger than the limit....if u dont mind can u give me u eamil id so that i can mail u the ipt files and iam file

many thanks,

chris

[chris44]

okay...okay...

[chris44]

sorry....i need to type one more message to enter a link

[chris44]

never mind shift about the email id....i will post a link so that u can download it through rapidshare...
here is the link

http://rapidshare.com/files/302083704/New_WinRAR_ZIP_archive.zip

[shift1313]

sorry chris, i didnt have a chance last night to play with this. did you make any progress on it?

[chris44]

hai shift,

thanks for replying....yes i did some progress....actually when i applied some torque....it is revolving and iam getting the desired elliptical shape

but it says my mechanism is over constrained by 2 dof's.....i am not sure how to fix this things....if u dont mind can u please check the model....and give me some suggestions how to fix these overconstrained dof...

i have send the files to ur email id.....(both ipt and iam)

thanks a lot shift,

chris

[shift1313]

chris, i dont have anything in my email. can you attach a screen shot of your design tree with all the joints and grounded components in it? Which components does it say are over constrained?

[shift1313]

When i open the file up in dynamic simulation it says it is over constrained by 1. The issue is the sliding on plane joint. The problem is when you create this joint(or its auto-created) you are not telling the roller that it can only slide in that groove. You are telling it that it can slide anywhere in that plane. Well the redundancy is the fact that your geometry only lets it be in that plane to start with so you are not accomplishing anything by placing this joint. If you simulate this, then suppress the joint and simulate again it will be an identical scenario.

I think one of the issues came about with your Mate for part7 to part 11. It appears as though you picked the center point of the circle rather than the face. This lets your "roller" spin around as long as its center point is located on that face. I suppress this mate and created another one in its place. When you go back into dynamic simulation this should take care of the issue with this component.

Is there another component that is having problems?

[chris44]

hai matt,

actually i updated the model....i am giving the rapidshare link....in this model...it says there are 3 unconstrained dof's....

can u please check on the model and give me some suggestions

http://rapidshare.com/files/303047697/New_WinRAR_ZIP_archive.zip.html

thanks a lot matt,

chris

[shift1313]

okay chris, its the same problem I stated above. Planning out constraints and joints needs a lot of attention. Its an interesting problem because you dont always need the same amount in the model as you do in real life. For instance when you bolt a part together, in real life you may have 8 bolts holding something together, but in the model, two insert constraints and one mate will accurately define the realtionship between the two.

The problem in you model is the same as with the last revision. The grey link in the image below is one of the issues. Its giving you an over constrained condition because the insert constraint for the pivot was created by selecting two edges. This selection makes both of these edges both concentric and planar. The "roller" has a tangent constraint with the bottom plane which is fine, but the mate between the side of the "roller" and the track is where the issue comes up. Now because the insert constraint gave this entire link a planar constraint, this mate between the roller and side of the track is not needed.

Another thing you need to be careful with is your selection for things like circular edges. If you select a circle with a green center point, you are actually selecting the center of the circle. If you right click or hover over the joint the "select other" will appear. this is a little icon with a green box in the middle and two arrows. the arrows let you select between different edges and the green box lets you finalize the selection. one of your joints was created with this which created an issue.


Basically I removed your constraints in the assembly and started from scratch. When you are in Dynamic simulation and you hover over a joint with a ! it will tell you the link that has issues. This doesnt mean you need to remove this joint, but some other joint is causing an issue for that one.

If you look at the second image you will see the mates i have in the model. I suppressed part C1 because it wasnt needed and was only adding joints to the model. The insert joint between the two components there i added a .15" offset which is how wide your part is.

Learning what joints you need is something you just have to look at and figure out unfortunately. This is why you should start with simple models first. Keep in mind the orientation of each part and what each mate does to it. In the assembly environment you can manually move things around and its a good idea to add a mate, move the model around to see how many degrees of freedom is still has. Play around with the selection process. edges vs faces vs points and so on. Hopefully this answered your question.

[chris44]

thanks a lot matt,

as u said, i removed the mate constraint between the roller and the slider...now its working great....i need to put more practice on placing constraints....and need to be really careful

[shift1313]

it just takes some practice chris. Building your models as you did is the way to go. Simple geometry without over-complicating things. Let me know if you need any more help.