Sorting contour entry / exit points

[bensls]

I have a lot of holes that I need to chamfer, and I like to use the center of holes as entry / exit points so the NC code moves the tool to the nominal location of each hole before plunging and circular interpolating.

 

Normally, I would just select the center point of a hole and then select the circle.  Then I'd check "use entry point" and "use exit point" under the Lead In/Out parameters.  

 

The problem I'm having is that the points in the chain manager don't sort along with the circles, and I don't have time to (and really don't want to) manually move each point before its associated circle.

 

Is there any way around this? 

 

I know I can just use a circle mill, but then I have to figure out the correct depth and negative wall stock.  Not the end of the world, but also not as simple as using the contour chamfer function.  Also, I wouldn't be able to specify my Lead In/Out line and arc.

 

I can also just abandon the entry / exit points altogether, but I like to see (and want my operators to see) the nominal hole locations in the NC code as a quick check to make sure they're all in the correct location.

[jeff]

Are the circles all different sizes? 

I never select the point AND the circle, just the circle for my 2D chamfers. 

[bensls]

Are the circles all different sizes? 

I never select the point AND the circle, just the circle for my 2D chamfers. 

 

The circles are all the same size in this case.  If you don't select the point, the toolpath will start at the beginning of the lead in line.  I want the toolpath to start at the center of the circle.

[Guest]

The circles are all the same size in this case.  If you don't select the point, the toolpath will start at the beginning of the lead in line.  I want the toolpath to start at the center of the circle.

 

Entering in the center for chamfering a hole is no big deal...just use your Lead In/Lead out to create a safe distance....

[bensls]

Entering in the center for chamfering a hole is no big deal...just use your Lead In/Lead out to create a safe distance....

 

Yeah I'm not worried about plunging into the part or anything.  Using Lead In/Out, you can get really close to the center of the hole with trial and error (or you can get virtually right on center if you want to do some fairly involved trigonometry to figure out the lead in arc length combined with the lead in line) but it's still not the same as simply using an entry point to locate directly at the nominal hole location.

 

My question is more about sorting linked geometry in the chain manager.

[Guest]

You are just over thinking it

[jaydenn]

Already answered.

[bensls]

You are just over thinking it

 

No, I'm not.  There is a perfectly reasonable explanation for wanting my tool to move to the nominal hole location before each chamfer operation.

 

It is possible to do this, but it involves placing the entry point before the contour chain in the chain manager.  I simply would like to know if it's possible to link these geometries so they sort correctly, or if it's possible to sort contour entry points at all.

[jlw™]

If I recall correctly the order doesn't matter. Hit the enter/exit at point and let it go.

[jeff]

No, I'm not.  There is a perfectly reasonable explanation for wanting my tool to move to the nominal hole location before each chamfer operation.

 

It is possible to do this, but it involves placing the entry point before the contour chain in the chain manager.  I simply would like to know if it's possible to link these geometries so they sort correctly, or if it's possible to sort contour entry points at all.

Yes you are, a simple equation will put your tool right on center of the hole when selecting just the circles.

(hole size - tool diameter /2) x .4142

 

Or circle mill will put it directly on center, and if it's a 90 deg chamfer tool, then the math is easy also. 

 

But afaik it's not possible to sort the points like you're asking unless I'm totally misunderstanding your question.

[bensls]

If I recall correctly the order doesn't matter. Hit the enter/exit at point and let it go.

 

Tried that already.  It's a mess.  The entry points just don't coincide with their respective circles.

 

Yes you are, a simple equation will put your tool right on center of the hole when selecting just the circles.

(hole size - tool diameter /2) x .4142

 

Well, I don't know where ".4142" comes from or where you want me to put that information.  But I could use the equation (hole size - tool diameter) / 2 if I were just using an entry line with no arc.  But I want to use an arc.

 

Or circle mill will put it directly on center, and if it's a 90 deg chamfer tool, then the math is easy also. 

 

That's what I've been using as a workaround.

 

But afaik it's not possible to sort the points like you're asking unless I'm totally misunderstanding your question.

 

That is exactly what I'm asking.  So I'll just assume we've reached a consensus that it is not possible to sort contour entry points and I'll continue using circle mill instead.

[BrianP.]

 

Well, I don't know where ".4142" comes from or where you want me to put that information.  But I could use the equation (hole size - tool diameter) / 2 if I were just using an entry line with no arc.  But I want to use an arc.

 

 

It's a formula that some one figured out a long time ago. The only thing Jeff forgot was a 135 degree sweep for angle . So for a .737 hole using a 3/8 endmill it's .737-.375 =.362 / 2 = .181*.4142 = .0749702. That is your lead in lead out for line and arc with a 135 sweep you will always go to center of a hole. Also handy for slots and a few other things where your sweep is tight. A little math for a 45 and you can bang it right on center or at least within a minuscule amount that your operators should be comfortable.

 

 

 

 

[Jayson Kramer]

No you cannot just sort the the center points in a contour and expect it to know what circle to go with. As really there are no options like drilling to sort. you can move the picking around in the chain manager if you want simple drag.

Now what almost all of us are not sure is, why you have to start at center as it still has to lead in and out based on entry and exit on the contour. but as I have found doing this and working with a lot of company's that there are people that want things go  a certain way so they make happen.Even though it really does nothing for the cuts.

[jeff]

 why you have to start at center

He mentioned that he wanted to start at center so his operators knew the location of the hole or something to that affect.

[jeff]

It's a formula that some one figured out a long time ago. The only thing Jeff forgot was a 135 degree sweep for angle . So for a .737 hole using a 3/8 endmill it's .737-.375 =.362 / 2 = .181*.4142 = .0749702. That is your lead in lead out for line and arc with a 135 sweep you will always go to center of a hole. Also handy for slots and a few other things where your sweep is tight. A little math for a 45 and you can bang it right on center or at least within a minuscule amount that your operators should be comfortable.

 

 

Capture.PNG

 

 

Capture 2.PNG

Yep, totally forgot about the arc sweep. my bad.

[bensls]

It's a formula that some one figured out a long time ago. The only thing Jeff forgot was a 135 degree sweep for angle . So for a .737 hole using a 3/8 endmill it's .737-.375 =.362 / 2 = .181*.4142 = .0749702. That is your lead in lead out for line and arc with a 135 sweep you will always go to center of a hole. Also handy for slots and a few other things where your sweep is tight. A little math for a 45 and you can bang it right on center or at least within a minuscule amount that your operators should be comfortable.

 

Ah okay.  That's what I meant earlier when I said it could be figured out with some trigonometry.  I should have known someone had already done the math and made it into a simple equation.  Thanks for clearing that up.  I'll definitely keep that constant handy.

[Colin Gilchrist]

As others have stated, just use Circle Mill for this, since you can get your Lead In/Out exactly how you want it, in addition to always starting at the hole center. Sorting will work on the Arcs selected this way, and you get the best of both worlds; the center start point you want, and the Lead In/Out. Plus, you don't have to mess with "chaining" the entry points. You do get to specify you Lead In Arc Size, and I would recommend just turning on "Perpendicular Entry". This gives you a plunge move at the center of the hole, a feed move perpendicular to the start point of the lead in move, a lead in line that is "perpendicular" to the entry arc (for turning on Cutter Comp, if you want to use it.) You even get the "Overlap" option to spread out the start/end point of the cut.

 

As for not having the "chamfer" options, yes that is annoying and I wish they would add that option to Circle Mill, so we wouldn't have to calculate the proper depth and negative stock values. But, if you go to the work of doing that, then just Save the Operation to an Operation Library. Then you can just "import" the operation, and you can even have the tool associated to the operation import with it. Pretty soon, you'll have a library of different Chamfer Sizes, associated to the Tool that works for that size. It is a simple matter to just Import the operation, window select (or pick your selection method of choice), sort the points, and regenerate.

[BrianP.]

Ah okay.  That's what I meant earlier when I said it could be figured out with some trigonometry.  I should have known someone had already done the math and made it into a simple equation.  Thanks for clearing that up.  I'll definitely keep that constant handy.

 

After a little more thought and research the formula that should work is take your tip dia. + your tip offset X 2 and use that for your diameter.

 

So on a half inch hole with a 1/4 chamfer mill with a .06 tip amd .03 tip offset you would have:

 

  .06 (tip dia. in tool definition)  +.06 ( tip offset x2 )= .120

.500 -.12 = .38 / 2 = .190 * .4142 = 0.078698

 

That in your line  and arc with 135 sweep will hit the center of the arc. Tried it for 3 different tools and worked for each.

[Newbeeee™]

Entering in the center for chamfering a hole is no big deal...just use your Lead In/Lead out to create a safe distance....

I do this and not worry about it.

And anyone on the machine who is reading code means the machine isn't cutting parts...

[jlw™]

This is driving me nuts and I can't get behind a keyboard. Some one make a bunch of arcs with points in the center then window select chains and see if it sorts the points for you.

[BCW]

This is driving me nuts and I can't get behind a keyboard. Some one make a bunch of arcs with points in the center then window select chains and see if it sorts the points for you.

 

Sorted fine using window select.

[jlw™]

I knew it would!

[bensls]

The arcs sort fine.  The points do not.

 

Unless that is a new feature in 2017.  I'm running X9.

[Jayson Kramer]

Ok so I created a bunch .5 dia holes . then I went to Chook and used Drillpt.dll to create points in the center of all dias.
Then went and selected contour and set it for chamfer and then set it to use start and end at point. worked great for all holes as you want.

[Jayson Kramer]

Here is what the chaining manager looks like.