HELP - Cutter compensation for helix bore toolpaths!

[colton_m]

Hi everyone,

I am here again in hopes someone can save me before I literally rip my hair out...

I am trying to preform a simple helix bore toolpath to expand a 1.250" Drilled hole to 1.408".

Under parameters when I select computer compensation everything works fine! However, it leaves no way to adjust at the machine for tool wear. When I select "Control" all I get is an alarm stating that "tool dia/nose R compensation start/cancellation is errenous" I can get the alarm to go away by setting the geometry and wear value in my machine to zero. However, again this defeats the purpose as it will not run with any other value other than zero!

I am using mastercam X2 to program a 3axis hitachi seiki mill (yasnac control). I am using the generic fanuc 3axis post. My tool is a 1" Indexible endmill.

Please, any help is apreciated!

Thanks,
Colton.

[Superman]

Helix bore with start off with an arc- your machine must be able to take up comp on an arc. I think the arc radius lead in/out will be 0.352"

"Control" means you have the place the tool radius into the control and your lead in/out must be larger than the tool radius

"Wear" means you set the tool radius to zero- ( +ive value in machine leaves that much material on the contour, -ive = cut deeper past the contour )

You may get better control using a 2D_Contour, and set the contour type to ramp- set the Ramp Options (!) to "Depth" - the ramp depth is the pitching down, turn on "Make pass at final depth", unselect "Linearize helixes", comp type to "Control"
You can also play with "Lead in/out" so comp can be taken up on a line ( lead in, try perpendicular line 0.352", lead out, perp line .05", arc sweep 45, radius 0.65" ) ( my lead outs may need adjusting )

[mxer]

I would say your lead in needs adjusting to accomodate your cutter comp. Or you could use computer wear and adjust hole size by changing stock to leave in Mastercam.

[colton_m]

Alright,

I tried using "Wear Compensation" again, with the tool radius and wear value set to zero it runs. When I change the wear value at the control to anything other than zero it stops with the same "tool nose R / diameter compensation start up / cancellation" alarm...

Any ideas as to why this is happening?

I am going to try the "Control Compensation" right now and see if that works... How can you adjust the length of the lead in/out for a Helix bore toolpath? In my case I don't think it is larger then 0.500"!

Thanks

[mxer]

It sounds like maybe you have too much cutter comp on tool to be able to turn it on. Like not enough room in hole to turn it on. Try adjusting your tool diameter in Mastercam by .0001 and see if this works. I've ran into this before on our Mori's but it has been a while.

I always have start on center checked when helix boring. You may have better luck as said before with 2d contour with ramping on or by using the circle mill path.

[colton_m]

UPDATE:

using 2D contour with ramping on is working flawlessly, Helix bore is still useless at this point.

[Superman]

Helix bore is not too good if you want cutter comp ON, either using "Control" or "Wear"
You do not have any control over the lead in / out and the leads will all be arcs ( no lines at all to take comp up on )
Like I said in the earlier post, the lead in arc will be max 0.352, to use "Control" the maximum tool dia is 0.704", so you would use a 5/8" cutter

This strategy is great for hogging the material out while not using comps
then come in with a finishing strategy to complete the shape to size ( with comps ON )

Using 2D_contour with/without the "Ramping" is what you want to use in it's place

[cadcam]

use helix bore but use start at center and add the option to move perpendicular to. this will give you the liner line of code so the machine will comp. do all the time.

[ObrienDave]

There are a lot of controls that will NOT do cutter comp when the first and last move is an arc.
Try adding a short straight line move at the lead in/out parameters page.
If you are using edge programming then the radius MUST be larger than the cutters radius plus the cutter comp value.
If you are using centerline programming then the radius must be larger than the cutter comp offset you are using.
Especially if the cutter is LARGER than the one you programmed.
That is probably why you are receiving that particular error message.