revolute joint issue

[Anonymous]

I need your help again.  In the past, I was able to create a revolute joint and have it work .  Now, although it appears that I can create the revolute joint, when it spins, the vertical post does not move.  The vertical post should rotate as the revolute joint moves.  

What am I doing wrong?

I appreciate your help.  

[Anonymous]

@Anonymous

It looks as if you accidently created a joint origin in the root-component and not in component2. Then you used this joint to create the rigid joint of component3?  As a result component3 does not follow the rotation of component2.

Manfred

[Anonymous]

Danke Manfred.  This seems like a simple solution.  However, there was not enough meat on it for a beginner such as myself to grasp.  I have now activated each component when I made the joint origin and the vertical still does not rotate.  Please give more details on exactly how to do this.  I have not found on the web how to do this.  Please see attached.

I appreciate your help.  

[Anonymous · Accepted solution]

@Anonymous

Upps, sorry - but for me, the clever way you parametically positioned the joint origin tangent to component2 did not look like the work of a beginner....so I thought you just missed/forgot one little action, that I occasionally also miss. So I just wanted to give you a quick hint.

Now more detail. Most important: you did the difficult things right, no need to change.

And I don´t have to explain how you can create your "joint origin1" - you already did that: tangent construction plane, sketch on construction plane, add point and then create a joint origin on that point. Then you used this joint origin for positioning of component3! Great!

Only one small correction is needed. You created "joint origin1" in the root component. But you have to do this in component2!

So please delete "joint origin1", construction plane and the sketch you used for it (brutal, but I don´t want you to mess with the timeline stuff - not now).

Then, activate "component2". This is the only difference to what you did before! And create a joint origin in exact the same way you did that before: tangent construction plane, sketch on construction plane, add point and then create a joint origin on that point.

Then use this joint origin (which is now included in component2) to position component3 (as you did before).

hope this helps

Manfred

[Anonymous]

Well Manfred, I believe that we are making progress.  I understand that I do not understand hierarchy!  I thought that I followed the steps that you described, but it did not work.  I will again emphasize that I really am a beginner despite your complements.  What I need is a step by step.  If you can suggest a URL for me to watch, I can do that instead of forcing you to go step by step.  You can see from my new file that I still do not have it even though I thought that I was following what you said. 

I do appreciate your help.

Marilyn  

[Anonymous]

Marilyn,

to be honest, I feel a bit helpless and also confused (I can see that you provided 7 accepted solutions to problems of other users - which seems quite a lot for a "beginner").

If you have problems to understand fusion hierarchy (bodies vs. components, rule #1, assemblies), maybe you should first work on this, you definitely need to have a good understanding regarding these subjects before you continue - there are plenty of sources if you enter these search subjects.

regards

Manfred

[davebYYPCU · Accepted solution]

Something like this one?  Another way to get things done.

You don't follow rule 1, as intended, 

The problem comes from Sketches that are not inside the components.

the Joint origins - only need one, where the pin is to sit.

The pin sitting tangent is ok for welding the two components, but I inserted the pin to the axis in the case you want to combine cut the socket.

Create Component and activate it, make the parts on the origins, reduces the need for Joint Origins, then assemble them,  

Step by Step up the time line, compare to your file, 

Edit the Joint limits, if the Animation is not what you are after,

file attached....

[TrippyLighting · Accepted solution]

Before attempting to create assemblies and joints you should first refresh Fusion 360's R.U.L.E #1. 

In short instead of first creating sketches and then creating components from the resulting bodies, first create empty components and make sure that they are activated.
that will keep the sketches for these bodies in these components.

You created several joint origins I am assuming to create joints. I did there same thing when I started with Fusion 360. However, only in rare cases are explicit joint origins really necessary.

Once you start to create a joint the necessary joint origins will be created on the fly.

[Anonymous]

Thank you Dave.  I can follow this!  I do have a couple of questions.  

What is the purpose of sketching a circle on the midplane between the two boxes that are on the base?  

Why did you ground?

How did you get the joint origin inside the axle?

This was great!  I appreciate your help. 

[Anonymous]

Thank you Peter.  Once again, I appreciate your help.  I did not know about creating empty components and then creating within them.  I did recognize the document that you recommended; there is so much information concerning Fusion 360 and it does not all stick!  Thank you! 

[davebYYPCU]

What is the purpose of sketching a circle on the mid plane between the two boxes that are on the base?  

No that is the joint origin for the base, made by Origin between faces, by coincidence is on the origin plane of the Model, but there is no sketch there.

Why did you ground?

So the base won't spin around the axle,

How did you get the joint origin inside the axle? 

This is done with a sketch on the axle origin plane, project the end of the axle, then a centre line, dimension the line for distance to centre of pin.

Axle Joint origin goes on the end point, of the line.

Pleased you can follow it....

[Anonymous]

David, I

I appreciate your help.  

You wrote:

How did you get the joint origin inside the axle? 

This is done with a sketch on the axle origin plane, project the end of the axle, then a centre line, dimension the line for distance to centre of pin.

Axle Joint origin goes on the end point, of the line.

I drew the line on the end of the axle, and then one from the center to the inside of the axle several mm in (looks like yours).  I was able to put a joint origin off the end of the axle and then move it in to where the internal line ends.  However, I was not able to get the join origin to lay down, so when I create the joint, the pin sticks into the end of the axle.  How did you get the joint origin to lie down?  

[davebYYPCU]

In my example, it arrived in the correct orientation, or Fusion put it there for me, I did nothing special, 

my sketch was on the Origin plane that I wanted the Joint Origin to lay on, could be you are on the vertical plane with your sketch, would look the same,

but putting then then moving the Joint Origin sounds odd,

can you place it directly, by hovering the mouse over the End point?

For now... I want to find a link I saw about this, operation....

[Anonymous]

Dave, this is a mystery to me.  I know how to draw on only plane, but I don't know how to draw with respect to the axle.  I know how to draw on a tangent plane to the axle, but that would be on the top of the axle, not inside the axle.  Exactly how did you do that please?

I appreciate your help.

[davebYYPCU]

Ok, did a screencast for this, but got a little long winded, sorry about that,

included some techniques using the Origin/s I find helpful....

and happy to answer questions...

[Anonymous]

David,

Thank you for your generosity giving me all this time.  The screenshot was very instructive.  One issue.  I can click on the plane that you indicated, but I can not figure out what to do next.  I cannot get those lines at the end of the axle when I am working on that plane.

I appreciate your help.

[davebYYPCU]

Yep, I didn't explain that, 

Can you confirm that you have a copy of my file to edit if you wish to?

It is all about the little yellow light bulbs.  Hide and show.

Activate the Axle Component, Hide the axle body, the Pin and Base components

After creating the new sketch it is for the Joint Origin in the axle, Show the axle with lightbulb on, 

So the first thing in the sketch is 

Sketch > Project > Project Intersect - ( in this dialogue box, two options, Objects or bodies icon, select Objects not bodies - will make sense soon)

left click on the face end of the axle - you will get the purple line, click Ok in the box.

Hide the axle with lightbulb, again,

Make a line from mid point of purple line, (mine is 7.5mm long, and perpendicular constrained.)

Stop sketch.

Next, make the Joint Origin on the End Point of the black line.

Trick is to hide and show - what is in the way, hide, what you need or what you are doing, show.

[Anonymous]

Dave, I am so appreciative that you have been willing to spend the time to help me.  I very much like your elegant solution, and I would like to use it.  

------- 

Wow!  I was able to follow what you did on your file.  I ran into a snag when I tried to repeat it  myself.  

Activate the Axle Component, Hide the axle body, the Pin and Base components   I DID THIS.

After creating the new sketch it is for the Joint Origin in the axle, Show the axle with lightbulb on, 

So the first thing in the sketch is 

Sketch > Project > Project Intersect - ( in this dialogue box, two options, Objects or bodies icon, select Objects not bodies - will make sense soon)    THERE WAS  NO OPTION TO CHOOSE OBJECTS OR BODIES; THERE WAS AN OPTION TO CHOOSE ENTITIES OR BODIES.  

left click on the face end of the axle - you will get the purple line, click Ok in the box.   WHEN I HID THE BODY OF THE AXLE IN THE ACTIVATED AXLE, THERE WAS NO FACE TO CLICK ON; THE AXLE WAS GONE.  

[Anonymous]

@Anonymous

Just in case that you are really interested in saving your time by understanding what you are doing with Fusion (and not just follow some clicks): Fusion has a nice help:

-> click on the "i"

-> this brings up this little window

and clicking "More Information" brings you to the "Learning" page of Autodesk with a lot of information and reading.

or....you can call Jamie......

[davebYYPCU]

Yes Entities, not Objects, in that dialogue box, 

My point there was not to use Bodies,

that option will Project a rectangle, by click on the body at any part of the body.

To click on the end face of the axle, you need to see it, you missed,

Show the axle 

before using the projecting command.

Earlier you could not start the sketch on the Origin plane because that axle is in the way, 

It's all about using the light bulbs, to see and hide what you need, for clarity,