Wear comp with tools near hole size

[SSS824]

I have been trying to get my Doosan to not alarm when using wear comp to threadmill a 3/4-10.  The hole size is .656" and the threadmill is .495" I know to engage wear comp normally a move of .2475 or more is required.

 

Is there a way to engage comp above the hole or some other way of approaching this?  I use wear comp all the time, but not on close fit holes even though I would like to.

[JParis]

Wear comp can engage with as little as a .001" move....control comp requires minimum of half the dia

Wear should not be a problem

[SSS824]

10 minutes ago, JParis said:

Wear comp can engage with as little as a .001" move....control comp requires minimum of half the dia

Wear should not be a problem

I get an alarm ps0034 only G0/G01 allowed in stupid/ext blk

[JParis]

What control? Machine?

[crazy^millman]

19 minutes ago, SSS824 said:

I have been trying to get my Doosan to not alarm when using wear comp to threadmill a 3/4-10.  The hole size is .656" and the threadmill is .495" I know to engage wear comp normally a move of .2475 or more is required.

 

Is there a way to engage comp above the hole or some other way of approaching this?  I use wear comp all the time, but not on close fit holes even though I would like to.

That is not wear comp that is Radius comp huge difference.

[SSS824]

I think I needed to select perpendicular entry in lead in/lead out..I see it puts a small linear move in before the g41.

[SSS824]

Deselecting start/end at center allows me to input a .001 entry/exit line length..but then the toolpaths retracts out of the hole after every pass WHAT!

[AMCNitro]

Ive had this problem  when I worked a shop that had Doosans.  Haas machines have the same problem as well.  You cant activate tool comp with a radius entry, it needs to have a straight entry, then the radius.  

[AMCNitro]

That's how I do it for the Haas.  Making molds now, and I thread mill everything.

[SSS824]

32 minutes ago, AMCNitro said:

That's how I do it for the Haas.  Making molds now, and I thread mill everything.

There are a lot of silly if/then things with machining because everything hasn't been updated since 1970..but we have to use what we have, thanks for the help.

[cam-eleon]

draw in a small entry move at your contour start and check these in the lead in/out. Test is as i don't normally use this feature but I think it turns the comp on above the contour

 

[Leon82]

Set entry exit arc clearance lower. 

 

Mine are at .005 to .01.

[crazy^millman]

Re read the 1st comment. With wear comp you don't need to move at least the radius of the tool. That is control comp and this topic wrong and the wording in it is wrong. He might be adjusting the wear value, but some where on the machine they are putting in a Radius value in the control for the tool. That right there is a big red flag. I will normally start at Zero with wear and then adjust from there. Not the radius of the tool that means CONTROL COMP not wear.

[SSS824]

1 hour ago, 5th Axis CGI said:

Re read the 1st comment. With wear comp you don't need to move at least the radius of the tool. That is control comp and this topic wrong and the wording in it is wrong. He might be adjusting the wear value, but some where on the machine they are putting in a Radius value in the control for the tool. That right there is a big red flag. I will normally start at Zero with wear and then adjust from there. Not the radius of the tool that means CONTROL COMP not wear.

Turning on wear comp in Mastercam, I don't enter anything for the endmill size at the control.  On the wear offset page I enter a -value to cut more from the ID I.E. -.002" for most endmills to cut on size as they are ground .002" under.

 

I have been using it for years this way.  I think it was more of an issue of getting Mcam to output the linear movec before comp in a threadmill cycle without making odd moves.

ACnitros picture of his settings are what I needed to use.  Playing around with start at center and end at center do cause an odd thing though.  The tool does one helix as expected, then retracts out of the hole and then re enters.

[SSS824]

What I can't figure out now is how to get the lead in to enter the cut smoothly, it is going straight down into the material and then interpolating.  Perpendicular entry gives wear comp the small linear move it needs, but then you lose the gradual entry into the cut.

Attached are the beginning moves of the cut.

Wear comp works but terrible entry into cut.

_______________________________________________________________________________________________________________________________________________________

This is smoother entry but lose wear comp

[SSS824]

This setup gives the best control over making a linear move first, as well as a smooth gradual entry into the cut.

But it retracts out and back into the hole every pass for some reason??????

If that could be disabled somehow I would have exactly the control I am looking for over the tool. 

 

[gms1]

 

This is my 5/8-11 threadmill cycle settings. I never turn on perpendicular entry. if they need to comp larger than that .020" value I change the major diameter of the hole to compensate (and yes some machines just suck at making threads so sometimes I have to adjust that).

 

FYI those feeds and speeds are what we use on welded a572 plate.

[SSS824]

17 minutes ago, gms1 said:

 

This is my 5/8-11 threadmill cycle settings. I never turn on perpendicular entry. if they need to comp larger than that .020" value I change the major diameter of the hole to compensate (and yes some machines just suck at making threads so sometimes I have to adjust that).

 

FYI those feeds and speeds are what we use on welded a572 plate.

Your settings are outputting a move straight down in Y fully enveloping in the cut.  I prefer not to do this especially if I am doing 1/4-20 x 1.000 deep in stainless etc..snap city.

[gms1]

It never snaps. And this is for a 5/8-11 not a 1/4-20 1" deep in stainless.

[JParis]

Heck, I'm threadmilling some 1-72 holes in titanium at the moment...pretty stout tools

[SSS824]

Just now, gms1 said:

It never snaps. And this is for a 5/8-11 not a 1/4-20 1" deep in stainless.

But I am trying to find the absolute best Mcam setting for difficult holes not easy ones. 

Try these parameters and watch it run, it has a very smooth entry, but it retracts out of the hole like a glitch.

[JParis]

Just now, SSS824 said:

but it retracts out of the hole like a glitch.

Not a glitch, it works as designed...

Been over this with CNC

[SSS824]

1 minute ago, JParis said:

Heck, I'm threadmilling some 1-72 holes in titanium at the moment...pretty stout tools

In one pass too I bet 

[SSS824]

Just now, JParis said:

Not a glitch, it works as designed...

Been over this with CNC

If you could elaborate we might be on to something.

[JParis]

1 minute ago, SSS824 said:

If you could elaborate we might be on to something.

It clears the hole....multi-passes, it clears out of the hole...you can certainly log onto the CNC Software Forum and bring it up again

Not 1 pass on that threadmill...only has 3 threads on it, so it's a couple passes