Making a rod end bearing need help

will_aldridge

I'm new to this and not even sure how to phrase this.  I've been using Rhino for the past 9 years and I recognize this user interface as being vastly superior but it's confusing me no end right now.  

I started off trying to make a rod end bearing (I titled it mm-4 Rod end bearing) for those who would like to take a look at it.  As you can see I have the general shape created and I have sketched in the ball portion of the bearing but I after that I'm lost.  I want to subtract the ball area from the main housing and then add the ball itself.  I can make a surface for the ball but I think I want a solid.  Any help is appreciated.  

nav

Hi @will_aldridge hope this helps you, sorry I did not use words to describe ii sometime is faster this way.

3dcad

Can you please share link to your document if you have made it public?

erwin_1

Have a look at mm-4 Rod end bearing - Copy.
First, you don't need sketch 2 (I suppressed it).
For the end piece: you can make the extrude symmetric. So you don't need the mirror. 
The rod itself, if you make your sketches closed you can rotate them to solids. I added the rod with the end piece directly in the revolve.
The ball itself: it's impossible to make a full rotate of a full circle. One has to use a half circle. I did this by adding a centre line in sketch 3 and then a revolve.

The resulting ball (part 2, tool) was subtracted from part 1 (subject), don't forget to select 'keep tools' in this case.

HTH

will_aldridge

erwin_1 said:

Have a look at mm-4 Rod end bearing - Copy.
First, you don't need sketch 2 (I suppressed it).
For the end piece: you can make the extrude symmetric. So you don't need the mirror. 
The rod itself, if you make your sketches closed you can rotate them to solids. I added the rod with the end piece directly in the revolve.
The ball itself: it's impossible to make a full rotate of a full circle. One has to use a half circle. I did this by adding a centre line in sketch 3 and then a revolve.

The resulting ball (part 2, tool) was subtracted from part 1 (subject), don't forget to select 'keep tools' in this case.

HTH

Thanks that helped quite a bit but I have some questions:

The symmetric part helped I didn't know about that.  

The revolve for the threaded rod portion I'm not sure how you did that because when I try and close the sketch it adds the half of the rod to the end housing and extrudes the whole thing together.  

Sketch 2 is the actual cross section of the ball, so that's what I want instead the solid blue ball depicted in your drawing.  So do I have to do that (make the ball in order to carve out the housing) then delete it and go back and revolve sketch 2?

Thanks again.

nav

Hi @will_aldridge hope this helps you, sorry I did not use words to describe ii sometime is faster this way.

andrew_troup

The print gets scaled a bit small in his excellent presentation, but a key step in @nav 's Boolean operation, in which he subtracts the ball from the housing, is "Keep Tools",. This saves you having to go back and recreate the ball after using it as a "tool" to create a matching cavity.

nav

andrew_troup said:

The print gets scaled a bit small in his excellent presentation, but a key step in @nav 's Boolean operation, in which he subtracts the ball from the housing, is "Keep Tools",. This saves you having to go back and recreate the ball after using it as a "tool" to create a matching cavity.

Thanks Andrew for pointing this out is very important indeed, in the video it might not be very visible.

will_aldridge

Yeah that helped a lot.  Thanks.

gonzalo_chomon

@will_aldridge, I created a couple of standar rod end bearing (ball joint) series SAK and SQZ here is the link to the public documents I have created two sizes of each, you can create more just changing the sizes on the sketchs, the specs of the series are in the same container:
SAK series: https://cad.onshape.com/documents/f52860ded70d4c05ad4b5e84/w/430ea3fc771b49ec83d73a38/e/c8e84a758d1e4e7fbf96ace5
SQZ series: https://cad.onshape.com/documents/1207b57818aa4b94b27769c1/w/fa82a0c600484208acadf9fd

Hope it helps.

will_aldridge

gonzalo_chomon said:

 you can create more just changing the sizes on the sketchs, the specs of the series are in the same container:

Hope it helps.

Thanks, I kind of had in the back of my mind that that would be nice if onshape could do that but I didn't know if it could and until I looked at your files I didn't realized that the whole housing was a revolve with the faces milled flat.  Or at least that makes construction easier, though I'm still struggling through figuring out how to cut off the faces with another solid.

andrew_troup

One easy way to "mill" off the opposite faces is to sketch a rectangle on a suitable (orthogonal) plane.
The rectangle should enclose everything you want to keep.
Then "Extrude/Solid/Intersection" (which is equivalent in other MCAD modelers to "Extrude/Cut/Flip side to cut")

The way to conceptualise this is that you're extruding another solid, and then preserving (effectively as a new solid) the volume which is shared by the original revolved solid and your newly extruded solid.

will_aldridge

One step forward 2 steps back it seems.  I didn't quite do it as elegantly as you described Andrew but you can see how I managed it.  I drew 2 rectangles and extruded them.  

Now for the 2 steps back.  I had managed to get the ball drawn and even mated it correctly so it would spin freely in the housing.  But after I went back and reconstructed the bearing ala gonzalo's method of revolving it now the ball doesn't show up in the assembly tab.  It's drawn in in the parts studio but I don't know what's keeping it from showing up in the parts studio, and obviously you can't mate a part that's not in the studio.  

 

andrew_troup

will_aldridge said:

One step forward 2 steps back it seems.  I didn't quite do it as elegantly as you described Andrew but you can see how I managed it.  I drew 2 rectangles and extruded them.  

Now for the 2 steps back.  I had managed to get the ball drawn and even mated it correctly so it would spin freely in the housing.  But after I went back and reconstructed the bearing ala gonzalo's method of revolving it now the ball doesn't show up in the assembly tab.  It's drawn in in the parts studio but I don't know what's keeping it from showing up in the parts studio, and obviously you can't mate a part that's not in the studio.  

 

Will - in the interests of clear communication, could you have another crack at the last sentence?
When I open your document, there is a ball "showing up in the parts studio" which seems to contradict both the last two parts of your sentence.

 Another tip:  it pays to avoid thinking of sketching, and the modelling effort it supports, as "Drawing", because that term is reserved (in 3D modellers) for creating 2D output.

will_aldridge

Sorry I meant assembly tab.  Both parts are in the parts studio but it is my understanding that the assembly tab is where mate operations are performed and since the ball isn't in the assembly tab I'm not sure how to proceed.  And I can't figure out why the ball isn't showing up there in the first place.

will_aldridge

OK I just figured out how to insert part 2 into the assembly tab.

andrew_troup

Will
If you're wanting to develop some good habits, you need to re-read (and apply) the advice from @nav above, and from me.

You've modelled several volumes twice, and you never need to do that in Onshape.
With the boolean options built into all Onshape solid creation features, you can model the ball, then subtract it from the housing and yet keep the ball

A similar philosophy applies to the "milling" operation.

However if you care only about getting a result regardless of how long it takes, and never intend to go back and edit a model, you will do just fine.

will_aldridge

I started from scratch and remade the whole thing: https://cad.onshape.com/documents/1dc2e291ede14902883ab02b/w/491b7cac1c3e4cc3b17f4f44
I just realized how to use a single box to "mill" the faces as you indicated Andrew but other than I I think the new version doesn't show any bad habits?
I do appreciate your corrections and i have tried to apply them.  The totally new interface just took some getting used to.

andrew_troup

will_aldridge said:

........ I think the new version doesn't show any bad habits?

Far from it. It looks entirely kosher to me. The only lapse from best practice which struck me can be laid at Onshape's door:

 it has named as "Delete Part 1" the feature which actually deletes Part 3 (of course, this reflects that it is the first occurrence of Delete Part in the tree, but it is confusing phraseology and if I expected to revisit the tree of a model where this had happened I would probably rename it to remove the ambiguity.)