CIRCULAR PATTERN

[ronneilbucago]

Need help making hole pattern in a circle direction of 4 different angles. Any idea how to do this in one shot? I've tried to play around using relations pattern but im not that familiar with the command...(mem_i, mem_v...etc)... Your help will be appreciated.....

 

[ronneilbucago]

[No message]

 

[zpaolo]

If you absolutely need to make it in a single feature, use a table pattern on the angle dimension that drives the angle between the hole and a datum plane.

 

[zpaolo]

If you absolutely need to make it in a single feature, use a table pattern on the angle dimension that drives the angle between the hole and a datum plane.

To be more precise, I sketched the hole as follows:



notice the centerline used to define the angle of the hole position. Then the pattern table, using that dimension as reference, is as follows:



I'm almost sure there are better methods (like axis patterning for 60

 

[ronneilbucago]

Thanks for that. I've tried table pattern for my first attempt but did'nt succeed when it comes to the angle of hole opposite the main hole feature. I've tried 0 and -180 but it keeps on duplicating the position of the main hole. You can try and see it yourself. It seems to be very basic at first look.

 

[ronneilbucago]

Thanks a lot zpalao. Got your point. Now it's okay .

 

[zpaolo]

I'm glad it was helpful, I also tried with multiple direction patterns in "rotate" mode, this works too, but you have to be careful when placing the first feature as the first radial pattern only goes into one direction.



The idea is having a pattern with 3 instances 6

 

[ronneilbucago]

hey zpalao, got any idea why 20 radial line is required for this hole circular pattern? My point is that centerline itself is sufficient to drive the angle pattern for the hole but it's not. Otherwise, hole position will duplicate and will not rotate,.. That's what I missed actually..

 

[zpaolo]

In fact 20 is not a construction line, it's only a distance between the hole center and the axis center, measured along the centerline. I suspect that if you dimension the center of the hole with respect to the datum planes the radial pattern will not work as the dimension will not be radial "in structure"... Can you post a picture of what you mean?

Paolo

 

[zpaolo]

In fact 20 is not a construction line, it's only a distance between the hole center and the axis center, measured along the centerline.

I did some tests, I already PM'd you, but for everyone else, it looks like if you have a construction circle to define the pattern of holes, you need to define the radius of the construction circle "along the centerline" and not the usual diameter dimensioning.

Paolo

 

[ronneilbucago]

I extruded a circle feature to make a hole cut and reference it to a construction circle w/ a dia 508 then patterned it using pattern table. it will pattern in duplicate position.

proper way is to use radial construction line as ref instead of a circular construction line. Table pattern will work just fine. Or you can use hole command and use pattern table. It will also work fine.

I'm just confuse why extruded hole w/ a circular construction ref isn't possible w/ table pattern.