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SPHERES IN ASSEMBLIES
- Thread starter jheal
- Start date
beachcomber
Mechanical
Reference planes and connect relationship between centre of ball and housing etc.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
beachcomber
Mechanical
Look in Help for Connect and select the "Connect Command (Assembly Environment)" option.
The example shows a connect between two spherical faces.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
The example shows a connect between two spherical faces.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
Hi,
if you don't have access to GTAC here is their suggestion
along with a different way to get it 'seated':
In the ball part add a sketch that matches the diameter of the hole that it
will fit into. Then use the sketch to apply a connect relationship.
- or -
In the valve part create a revolved construction surface that matches your
sphere and positioned to 'shut' the hole. Then in assembly connect the ball
to the construction surface of the valve.
dy
if you don't have access to GTAC here is their suggestion
along with a different way to get it 'seated':
In the ball part add a sketch that matches the diameter of the hole that it
will fit into. Then use the sketch to apply a connect relationship.
- or -
In the valve part create a revolved construction surface that matches your
sphere and positioned to 'shut' the hole. Then in assembly connect the ball
to the construction surface of the valve.
dy
beachcomber
Mechanical
jheal,
We're guessing at what you want to do - can you be more specific about the problem, then maybe we can give you a correct solution.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
We're guessing at what you want to do - can you be more specific about the problem, then maybe we can give you a correct solution.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
- Thread starter
- #7
thank you all for your help, but i still cant seem to get it. I have a sphere that needs to be assembled in between two cylindrical housings at which each end the ball cannot get out. I dont really care where inside it is, the ID of the housings are larger than the sphere. I just want it for an exploded view drawing to show where it goes.
jheal,
I would create a sketch as DY explained but I would use sketch lines that correspond to the axis between the two cylindrical ends. Create a line axis in the sphere sketch as well. You should be able to apply an axial align between all three components of this part of your assembly. This will also allow you to leave the ball under constrained if it is to move between the two cylindrical ends.
Jef
I would create a sketch as DY explained but I would use sketch lines that correspond to the axis between the two cylindrical ends. Create a line axis in the sphere sketch as well. You should be able to apply an axial align between all three components of this part of your assembly. This will also allow you to leave the ball under constrained if it is to move between the two cylindrical ends.
Jef
Jef,
the axial align will leave 2 degrees of freedom (vertical
movement, rotation) and thus will center the ball but will
not 'seat' it
The circle method will leave 1 degree of freedom (rotation)
but will 'seat' the ball.
So which method to choose depends ..
dy
the axial align will leave 2 degrees of freedom (vertical
movement, rotation) and thus will center the ball but will
not 'seat' it
The circle method will leave 1 degree of freedom (rotation)
but will 'seat' the ball.
So which method to choose depends ..
dy
beachcomber
Mechanical
Try this one -
In the part file create a co-ordinate system at the centre of the ball.
In the assembly file create a co-ordinate system at the centre of one end of the cylinder.
Use the 'match co-ordinate systems' method to constrain the ball. This will create 3 alignment constraints. Adjust one of them to offset the ball the required distance from the cylinder end.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
In the part file create a co-ordinate system at the centre of the ball.
In the assembly file create a co-ordinate system at the centre of one end of the cylinder.
Use the 'match co-ordinate systems' method to constrain the ball. This will create 3 alignment constraints. Adjust one of them to offset the ball the required distance from the cylinder end.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
- Thread starter
- #11
I love all the suggestions people are giving me. Making a sketch in the in the sphere is a great idea, but none of the assembly relationships recognize that I have a sketch. The coordinate system was also a great idea, but ive tried it before, and im still trying, but the match coordinate systems relation wont even let me choose a coordinate system. Im starting to think that i have an intellisnap problem.
beachcomber
Mechanical
I know this sounds simple, but do you have the co-ordinate systems displayed? Same applies for sketches
All you do with this command is pick the two systems - it's probably the simplest method of constraining in Solid Edge.
To get the 2 systems displayed RMB on the two parts and select 'Show/Hide Component >> Co-ordinate Systems'
Similarly for sketches.
In my last post I said create a system in the assembly file at one end of the cylinder - it may be better in the part file.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
All you do with this command is pick the two systems - it's probably the simplest method of constraining in Solid Edge.
To get the 2 systems displayed RMB on the two parts and select 'Show/Hide Component >> Co-ordinate Systems'
Similarly for sketches.
In my last post I said create a system in the assembly file at one end of the cylinder - it may be better in the part file.
bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.
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