What's new
What's new

Help! Grooving with a radius

LisaM0311

Plastic
Joined
May 11, 2020
Hello all. I’m new to haas, but not to machining. Been machining on Mazak’s for 15 years. Recently got a Haas. I’m having a hard time programming a radius at the bottom of a groove. I can get a chamfer at the bottom just fine. But adding a G02 and a R just alarms out. Was hoping I could add a picture of the print and program I have so far, can see how to do that. I’ll add the program below
G00 Z-.9942 F.01
G75 X .5905 Z-1.2175 K.05 I.025
G00 X 1.2
Z-.9642
X.9742
X.9342 Z-.9842
X.6305
G02 X.5805 Z-.1.0642R.04 (If I clear the G02 and
And R I get a chamf)
Z-1.2275
X.9342
X.9742 Z-1.2475
X1.2

Any help would be appreciated, no one here to ask questions too.

Lisa
 
your z axis difference is .080 and your trying a R.04..im not familiar with Hass but i think thats where you should start looking. its hard to tell what to adjust without knowing the controlling dimensions.

there are plenty of people here to help, ,welcome aboard!


BOOZE got it!
 
G02 X.5505 Z-1.0242 R.04


Your change in X needs to double the R value, Your change in Z is the R value.

Thank you, I was wrong on the Z once I changed that it started the radius on the graphics. But alarms out again. X double on the line before X. 6305
.5905 is my finish diameter.
I know that X is still programmed wrong, my way of thinking I’m trying to leave .01 for a finish pass so that why I had a X .5805

So I have G02 X.5805 Z-1.0242 R.04 I see a radius so that’s a plus. I’m just playing around trying to learn, we are slow so no better time to learn. Thanks for your help!

Lisa
 
G02 X.5805 Z-.1.0642R.04 (If I clear the G02 and ...

First off, you have a Z- .1.0642 (you have an extra decimal in your code.

Beyond that, I think Booze called it.
 
Good for you for trying to learn.
If your finish is .5905 and you want to leave +.01, your G02 X would be .6005 not .5805.

The X value for the previous line would need to be .6805.

If the arc can be fit between the X and Z values the control will execute it , but it may not be a 90 deg arc which is what I suspect you want.
 
Good for you for trying to learn.
If your finish is .5905 and you want to leave +.01, your G02 X would be .6005 not .5805.

The X value for the previous line would need to be .6805.

If the arc can be fit between the X and Z values the control will execute it , but it may not be a 90 deg arc which is what I suspect you want.

booze! I appreciate you! Thank you! My numbers were all wrong 🤦🏻*♀️ Why it kept alarming out after I had good numbers, my next line I didn’t have a G01. Was still going off the G02. how long have you been programming G code? It’s a whole new ballgame for me, but so rewarding Have a great day!
 
My numbers were all wrong ����*♀️
Hello Lisa,
Even when your numbers are incorrect (for the geometric shape you want to describe), using "R" Format Circular Interpolation will result in an arc move being completed successfully, provided that its geometrically possible for the Start and End Points specified to exist on the arc element. However, the resulting arc wont be as you intended it to be.

In any motion control, the trajectory of a circular (arc) move is calculated on the basis of a Centre Point, a Start Point, and the Angular Move between the Start and End Point. When the information relating to a Circular Move in a CNC program is given in terms of Start, End Points and Radius, the control has to calculate the Centre Point of the Arc to use in the generation of the Circular Trajectory. If when writing a CNC program, either the Start Point, End Point, or both are inadvertently specified incorrectly, if its geometrically possible, the Control will simply calculate the Arc Centre based on the data given and then generate the Circular Trajectory for the Incorrect Arc without raising an error.

In your listed program of your first Post, it was geometrically impossible for an Arc to be constructed through the Start/End Points and Radius given and therefore, an alarm was raised. In some way, its fortuitous that your Arc was impossible to create, because small errors when using the "R" Format, Circular Interpolation, often go unnoticed (no alarm raised when its possible to create an arc through incorrect coordinates). If the Arc is only to debur a corner, or as an unimportant blend radius, then it will not matter. However, if a profile containing Radius features is important, then the error may not be pickup until final inspection, or use.

Alternate to the "R" Format Circular Interpolation, is I,J and K Format (I and K for a normal Turning Centre). Using this format, the centre of the Arc is communicated to the control via Vector coordinates from the Start Point to the Arc Centre. If difference in Radius of the Start Point and End Point, relative respectively to the Arc Centre is greater than a tolerance preset in parameters, then an alarm will be raised. Accordingly, a not so obvious error is found before the part is possibly ruined.

Although nothing really wrong with using the "R" format (I choose not to use it), its worthwhile learning how to use the I,J and K Format.

Regards,

Bill
 








 
Back
Top