tangent mate for mating cylinder with intersecting planes.

lorne_2

Hi,
  I am fairly new to Onshape.  I am having trouble figuring out how to mate a cylinder with two different intersecting planes. Here is a link to my project.

philip_thomas

Ok - I wanted this one because it's a great learning opportunity  - that's a euphemism for 'complex'!

That means that you my reader will have to follow carefully and ask any questions.

Let's start at the end - i have built a working solution. I have no idea if this is exactly what you're looking for, but then again i am a sucky mind-reader - just ask my ex-wife.






Lesson 1 - Keep each level of assembly structure as SIMPLE AS POSSIBLE
Each assembly level should contain only a handful of parts and sub-assemblies. 
Things that are bolted together and move should be a separate sub-assembly.
This lesson does not affect the ability to mate these parts - but does make it much easier for someone else (and the creator) come along and understand what is going on.

Lesson 2 - Keep the mates at the subassembly level. The only mates at the current level should be those mates that define the degrees of freedom between the various subassemblies

Lesson 3 - Name the parts you create - An assembly of 'Part 1' makes it very difficult to work with

Lesson 4 - Try not to create redundant mates. Onshape mates are remarkably powerful and in many cases a single high level Onshape mate replaces 2 or 3 traditional low level mates. Do not eliminate one degree of freedom between parts A and B with a mate and then eliminate another degree of freedom between parts B & C. Chances are a single mate between parts A & C will be the ideal solution.

Lesson 5 - Don't repeat features unnecessarily - Instead of multiple 'Delete Part' features, use a single one.

Lesson 6 - There was no need to import the assembly multiple times and delete different groups of parts. A single Part Studio (use the 'flatten' option) would have enabled you to easily build the sub-assemblies. Again, there was no need to generate more than a single part studio.

Lesson 7 - Keyboard shortcuts rock! 'K' toggles the visibility of Mate Connectors (this will be important later )

Lesson 8 - Colors go a long way towards making an assembly easily comprehensible

Lesson 9 - Name your Mates. Easy not to do when you just created it and know exactly what its supposed to do. Later it won't be so obvious



Other than the above, what's the trick?

Well first - Yes Onshape has a 'Tangent' mate - but it's not what you may be thinking its for. Yes a traditional tangent mate could be used to position the pins in the 'V's. It would however take 4 tangent mates that are very expensive and fragile (meaning they could flip sides). This is not a limitation of Onshape, this is true of any CAD system using this low level mate type. In Onshape, tangent mates are used for allowing a mate to cross faces - think cam follower - 






Onshape uses 'Mate Connectors' (local coordinate systems) that are then joined together using mates.

The trick here is to create Mate Connectors as children of the two sides of the V blocks. These should be positioned such that their origins are at the centers of the pins - their positions therefore, are determined by the angle of the Vblocks and the diameter of the pin.

To do this we are going to 'Derive' the pin into each of the Part Studios that contains the Vblock halves. These pins are for reference only.
Next we create sketches that contain generic circles - one for each pin location.
These circles have a constraint to make them equal in diameter to the pin (if the pin diameter changes, the sketch (and in turn the locations of the Mate Connectors) will update).
The circles are also tangent to the 'Intersection' curves generated from the faces of the Vblock






Next - Mate Connectors are created at the centers of the circles with the Vblock designated as the 'owner' part.
Now whenever the block is used in an assembly - the location of the centers of the pins are always and readily accessible.




There are a plethora of possible mating strategies - the one shown in my sample doc is just one suggestion.
What you should note however is how much cleaner the Assembly Structure looks and how much easier it is to find the appropriate mates














I hope this helps and please feel free to ask any questions

https://cad.onshape.com/documents/58aca5b78105ed0f83967aba/w/18109cbd006a72f6d78e30bb/e/e4aeacf14403e8d7e1a53e0e

philip_thomas

Before Neil and 10 other people start working on this - i am building an answer

philip_thomas

Ok - I wanted this one because it's a great learning opportunity  - that's a euphemism for 'complex'!

That means that you my reader will have to follow carefully and ask any questions.

Let's start at the end - i have built a working solution. I have no idea if this is exactly what you're looking for, but then again i am a sucky mind-reader - just ask my ex-wife.






Lesson 1 - Keep each level of assembly structure as SIMPLE AS POSSIBLE
Each assembly level should contain only a handful of parts and sub-assemblies. 
Things that are bolted together and move should be a separate sub-assembly.
This lesson does not affect the ability to mate these parts - but does make it much easier for someone else (and the creator) come along and understand what is going on.

Lesson 2 - Keep the mates at the subassembly level. The only mates at the current level should be those mates that define the degrees of freedom between the various subassemblies

Lesson 3 - Name the parts you create - An assembly of 'Part 1' makes it very difficult to work with

Lesson 4 - Try not to create redundant mates. Onshape mates are remarkably powerful and in many cases a single high level Onshape mate replaces 2 or 3 traditional low level mates. Do not eliminate one degree of freedom between parts A and B with a mate and then eliminate another degree of freedom between parts B & C. Chances are a single mate between parts A & C will be the ideal solution.

Lesson 5 - Don't repeat features unnecessarily - Instead of multiple 'Delete Part' features, use a single one.

Lesson 6 - There was no need to import the assembly multiple times and delete different groups of parts. A single Part Studio (use the 'flatten' option) would have enabled you to easily build the sub-assemblies. Again, there was no need to generate more than a single part studio.

Lesson 7 - Keyboard shortcuts rock! 'K' toggles the visibility of Mate Connectors (this will be important later )

Lesson 8 - Colors go a long way towards making an assembly easily comprehensible

Lesson 9 - Name your Mates. Easy not to do when you just created it and know exactly what its supposed to do. Later it won't be so obvious



Other than the above, what's the trick?

Well first - Yes Onshape has a 'Tangent' mate - but it's not what you may be thinking its for. Yes a traditional tangent mate could be used to position the pins in the 'V's. It would however take 4 tangent mates that are very expensive and fragile (meaning they could flip sides). This is not a limitation of Onshape, this is true of any CAD system using this low level mate type. In Onshape, tangent mates are used for allowing a mate to cross faces - think cam follower - 






Onshape uses 'Mate Connectors' (local coordinate systems) that are then joined together using mates.

The trick here is to create Mate Connectors as children of the two sides of the V blocks. These should be positioned such that their origins are at the centers of the pins - their positions therefore, are determined by the angle of the Vblocks and the diameter of the pin.

To do this we are going to 'Derive' the pin into each of the Part Studios that contains the Vblock halves. These pins are for reference only.
Next we create sketches that contain generic circles - one for each pin location.
These circles have a constraint to make them equal in diameter to the pin (if the pin diameter changes, the sketch (and in turn the locations of the Mate Connectors) will update).
The circles are also tangent to the 'Intersection' curves generated from the faces of the Vblock






Next - Mate Connectors are created at the centers of the circles with the Vblock designated as the 'owner' part.
Now whenever the block is used in an assembly - the location of the centers of the pins are always and readily accessible.




There are a plethora of possible mating strategies - the one shown in my sample doc is just one suggestion.
What you should note however is how much cleaner the Assembly Structure looks and how much easier it is to find the appropriate mates














I hope this helps and please feel free to ask any questions

https://cad.onshape.com/documents/58aca5b78105ed0f83967aba/w/18109cbd006a72f6d78e30bb/e/e4aeacf14403e8d7e1a53e0e

lorne_2

Thanks, I just got back to this now, I will review once I have a chance.  Thanks for the in-depth reply!

lorne_2

And yes, you did read my mind correctly about my design intent!

lorne_2

I am trying this out for  myself now finally.  I'm having trouble figuring out how to define mate connectors on my sketch.  I had assumed I would have to exit out of the sketch and define the mate connectors in the assembly, but I can't figure out how to show the sketch on the assembly level.

lorne_2

I figured it out.  You need to define the mate connector from within the part workspace.  I was trying to do it in the assembly.

philip_thomas

^^^