I'm a programmer, not a mech eng. so bear with me...
If I have a "large" tube with a series of holes along it, say 9mm diameter...
I have another component (an 8.9mm solid cylinder) which should be inserted in those holes...
...how is the best way of doing it?
I thought about adding a work axis in each hole, but can't find an easy way of doing even that!
So how would you do it?
If I make a hole in a rectangular block it all works out, the toroid appears and I constrain the small 8.9mm to the axis of the hole in the block.
That does not seem to work with holes in the large tube.
Solved! Go to Solution.
Solved by JDMather. Go to Solution.
Dear Oransen,
depending on the geometry of your 3D models, you don't necessary need to add an extra axis in all the holes.
In order to provide you a good solution corresponding to what you are expecting, that could be very helpful if you could have the possibility to attache directly here the assembly and its components.
Many Thanks
Best Regards
@oransen wrote:
If I have a "large" tube with a series of holes along it, say 9mm diameter...
In the large tube part click Work Point and then right click and select Axis.
Select the hole cylindrical face and then the tube face.
I would pattern the holes using Rectangular Pattern (even if not rectangular as long as it is in fact some regular pattern) http://home.pct.edu/~jmather/SkillsUSA%20University.pdf place and constrain one component in assembly and then use Pattern Component.
What version of Inventor are you using?
The CADWhisperer YouTube Channel
Again, I'm not a mech eng. so don't laugh too much when you see the attached files.
I can constrain the small tube to the hole using Mate Constrain.
But I can't constrain the small tube to the hole using Insert Constrain.
Inventor 2013
I've realised that maybe my problem is that Insert wants a flat round hole, but a round hole in the side of a cylinder is not flat.
@oransen wrote:I've realised that maybe my problem is that Insert wants a flat round hole, but a round hole in the side of a cylinder is not flat.
You are getting it figured out. Insert requires circular edges. Circles are planar entities and the edge of the tube cut by a cylinder (hole) is not planar.
You are missing constraints and dimensions for your points in the large tube Sketch - I would use a construction line.
But there is a better way altogether.
Because you will want to use a Component Pattern in the assembly you should use a Rectangular Feature Pattern in the large tube part.
Create one Hole feature and then Rectangular Pattern.
In the small "tube" part you are missing geometry constraints in Sketch1 (horizontal, vertical, perpendicular).
Check lower right corner of screen when editing a sketch.
Once you ge the hang of this - Inventor should be automatically creating your geometry constraints.
Post back if you can't figure out how to do the Component Pattern in the assembly.
You will need Workpoints in each part as shown in attached to constrain - or simply use a Tangent constraint.
The CADWhisperer YouTube Channel
Thanks for the info, and the image. I'll try that method.
(I know the parts are missing a ton of constraints, but I was just interested in one point, how to constrain the tubes to the holes.)
I've got the workpoints solution working, but could you explain the tangent solution a bit more?
@oransen wrote:I've got the workpoints solution working, but could you explain the tangent solution a bit more?
Mate the axis of the hole to the axis of the pin. (I think you got that.)
Then and a tangent between the planar end face on the step of the pin and the cylindrical face of the tube.
Just like how the real parts would contact if assembled.
The CADWhisperer YouTube Channel
@oransen wrote:
(I know the parts are missing a ton of constraints, but I was just interested in one point, .....)
The point I was trying to make is that Inventor should be doing this work for you - no extra work for you, and in fact, will save you work down the road.
The CADWhisperer YouTube Channel
@Anonymous wrote:
@oransen wrote:
(I know the parts are missing a ton of constraints, but I was just interested in one point, .....)
The point I was trying to make is that Inventor should be doing this work for you - no extra work for you, and in fact, will save you work down the road.
I don't doubt it, but I'm a slow sort. I'll get there in the end! Thanks for the pointers.