I J error on Haas

[jeffrey001]

Using X4 with Haas controller

Today, I had a simple 1in hole for a press fit oil bushing in the center of a 8 inches diameter plate.

Use wear comp with 15% lead in/out out and wear at zero for the 1/2 end mill at machine.

Hole was .002 smaller, enter -0.001 for the wear in the controller and got this IJ error.

Wear at zero, pass, Wear at -0.001, error.

I sometime got this error from time to time but never found why.

Tried to play with lead in/out but no success.

So what I do is put a -0.001 in the matarial to leave on wall.

Is there a setting to change to have Mastercam let me know that before loading the program into the controller.

Also, is there a rule to calculate lead/out for small hole, like a 1in hole with a 3/4 end mill.


Thanks for any input, will be greatly appreciated.


Jeff

[Larry Dickman]

What toolpath are you using? Contour?
Your lead in/out must contain a linear move to correctly turn the comp on/off

You would be better off using circle mill or helix bore toolpath. Select start at center and perpendicular entry.

[cadcam]

in the control settings do you have it set for wear and do you have a linier move like Larry said?

[jeffrey001]

What toolpath are you using? Contour?
Your lead in/out must contain a linear move to correctly turn the comp on/off

You would be better off using circle mill or helix bore toolpath. Select start at center and perpendicular entry.

Thanks Larry,

Using contour ramp, Use 15% tangent and 15% radius for lead in/out.

Should I be using linear instead of radius, for lead in/out, never think about that

Mastercam output linear moves and I use filter on the finish pass.

I'm not use to go with helix, I don't always think to use it. Sometime I have small holes to cut and when I was using helix, on the lead out move, the cutter snap the small plug that was left in the center of the hole.

I can leave with this error as it does not happen very often but would like MasterCam to let me know when it happen so I do not get this error when the program is in the controller.

Thanks, Jeff

[Larry Dickman]

[QUOTE=jeffrey001;1088829]Thanks Larry,

Using contour ramp, Use 15% tangent and 15% radius for lead in/out.

Should I be using linear instead of radius, for lead in/out, never think about that


Yes, you must. How large of a linear move will depend on how big a difference you will have between your programmed tool dia and actual. If your only looking to make minor corrections, leave your radius at 15% and add a linear move of 10%.

[Superman]

Using contour ramp, Use 15% tangent and 15% radius for lead in/out.

Should I be using linear instead of radius, for lead in/out, never think about that

most CNC machines use the linear component to take up or cancel the cutter comp, the radius is to blend the cutting action onto or off the contour. The linear distance you input (in Mcam ) must be larger than the value you need to place in the machine (control) ie you want to comp the tool by 0.005", then you need to have a linear move of at least 0.0051"
There are a few machines that do allow comp to be taken up on an arc

Mastercam output linear moves and I use filter on the finish pass.

put the filter ON for all ops if possible, it will make your programs shorter, easier to read, and your machine will run smoother

I'm not use to go with helix, I don't always think to use it. Sometime I have small holes to cut and when I was using helix, on the lead out move, the cutter snap the small plug that was left in the center of the hole.

drill, or helix cut out the small plug before doing the wall.
Helical cutting is more reliable, as the end of the cutter is used, less flex is generated, holes tend to be more true ( no taper)

I can leave with this error as it does not happen very often but would like MasterCam to let me know when it happen so I do not get this error when the program is in the controller.

The error tends to be an endpoint error, from the start of the arc lead in to it's endpoint, most times when doing quasi-arcs ( very short arc sweeps )
I try to do helix cutting with a perpendiculr linear move only at the top, with a lead out arc sweep of 45° or 90° with a perp. linear move

[jeffrey001]

Thanks Superman.

What is the difference between using Helix instead of contour ramp?

Does the code (helix) will be smoother than the ramp code?

Thanks a lot, Jeff

[Superman]

What is the difference between using Helix instead of contour ramp?

Does the code (helix) will be smoother than the ramp code?

Thanks a lot, Jeff

I stated Helix as a 3 axis movement of the tool to cover both senarios

"Contour ramp" is different to to "Helix" in that the lead in/out is easier to control in the contour ramp op.
Helix has to played with to get the lead in arc small enough to force a linear move for comp take-up

Using the "Filter" allows code to have arcs output, this is what give smoother operation of the machine, as well as shorter NC code