Radius face groove

[Lee Yeomans]

Hi,recently started a new job and the boss has just put me on a Mazak integrex 400IV, I’ve never really used mazatrol before, so been chucked in at the deep end.
Would any of you kind people know the correct way to program a radiused face groove please? As it doesn’t help that the boss can’t find the correct programming manual for the machine. Hopefully the picture attached will give you some idea what I'm trying to machine
Thanks

 

[TAIWA NUMBA WAAN]

I would use a round carbide insert on an axial tool holder, such as a face grooving insert with a round tip. I don't see any other way since there is no flat at the bottom and the side angle is 90 degrees. If you don't have CAM, you can program that manually with a G2 or G3 arc.

 

[Lee Yeomans]

It is a 15mm(7.5rad) groove, and I have a radiused tipped tool like shown but it has a 6mm rad tip in it, just struggling to program it

 

[sinha]

R = 7.5 - 6 = 1.5

 

[michiganbuck]

I'm not the CNC guy but the likes of a Baldor carbide grinder can make a darn good special in a few minutes.

 

[angelw]

It is a 15mm(7.5rad) groove, and I have a radiused tipped tool like shown but it has a 6mm rad tip in it, just struggling to program it

You're better off Circular Interpolating the Groove than using a 7.5 Radius Tool. Even with a machine like an Integrex in good order, a form tool matching the radius of the groove is going to chatter. The Mazak Programming System will eat that so long as you have the Tool Description registered correctly. If you were to program it in EIA code, and not using Tool Radius Compensation, effectively, the radius being cut will be R1.5.

I would start at the outside of the Face Groove and profile towards the centre, as there is natural clearance on the inner side of the tool. Depending on the size of the Outside Radius of the Groove, you may get some interference with the tool on that side, but because the cross section of the groove is a Radius, you should be right with the type of tool shown in Post #2.

Regards,

Bill

 

[BT Fabrication]

Id be finding a cam program and doing it that way. Manually can be done but not familliar with it.

 

[Cole2534]

Hi,recently started a new job and the boss has just put me on a Mazak integrex 400IV, I’ve never really used mazatrol before, so been chucked in at the deep end.
Would any of you kind people know the correct way to program a radiused face groove please? As it doesn’t help that the boss can’t find the correct programming manual for the machine. Hopefully the picture attached will give you some idea what I'm trying to machine
Thanks

Not exactly what you asked but....the Mazak programmers group on Facebook has tons of users with these controls offering up different ways to do things. I'd poke around there as well.

 

[Panza]

I think I might have a programming manual. Will look for it later today. Can't remember how to do it in mazatrol without a manual anymore, too long ago.

 

[Panza]

Found the book. The book is for a smart control but I guess all basic Mazatrol is the same ?
- Choose "T.Groove" unit.
- Face
- Pattern: #1 (isoscles) is the one that has Radius/Chamfer and such.
- Pitch is for when you want more than one groove.
- Width is for the top of the groove.
- Finish is what you leave for the finish tool
I assume you can figure out the tool settings.
Shape settings:
- S-CNR: Top chamfers or Radiuses (press corner R menu key for R).
- Start point is OD groove at the top of groove.
- End point is bottom of groove, OD.
- F-CNR: Bottom R's or chamfers.

That should get you going.
I have a workbook for integrex too bu found no face grooving examples there.

 

[Lee Yeomans]

Found the book. The book is for a smart control but I guess all basic Mazatrol is the same ?
- Choose "T.Groove" unit.
- Face
- Pattern: #1 (isoscles) is the one that has Radius/Chamfer and such.
- Pitch is for when you want more than one groove.
- Width is for the top of the groove.
- Finish is what you leave for the finish tool
I assume you can figure out the tool settings.
Shape settings:
- S-CNR: Top chamfers or Radiuses (press corner R menu key for R).
- Start point is OD groove at the top of groove.
- End point is bottom of groove, OD.
- F-CNR: Bottom R's or chamfers.

That should get you going.
I have a workbook for integrex too bu found no face grooving examples there.

Cool thanks, will give it ago next time I'm in

 

[Philabuster]

I could program that groove in Mazatrol for you and post the info, but I need the print dimensions to help you.

Because the faces of the top of the groove are not on the same plane, the normal grooving cycle will not work. This needs to be programmed as a face contour instead.

 

[Dan from Oakland]

Regarding your insert, you may well need to give the insert more side clearance to prevent it from rubbing. Your inside edge may be ok but the outside edge may need to be relieved.

 

[Lee Yeomans]

I could program that groove in Mazatrol for you and post the info, but I need the print dimensions to help you.

Because the faces of the top of the groove are not on the same plane, the normal grooving cycle will not work. This needs to be programmed as a face contour instead.

Hi, sorry for the late response, that would be great thank you, what bits of info are you requiring?

 

[Philabuster]

Hi, sorry for the late response, that would be great thank you, what bits of info are you requiring?

The only information you provided it was a 7.5mm radius groove. I am assuming the depth of the face groove is also 7.5mm?

I need all of the diameters and lengths for the feature and also the radius tangent to the 7.5mm groove to help you out.

I would program this in two units. Turn the OD with a CNMG tool and then cut the face groove with your 6mm radius tool. Keep in mind, the 6mm tool will need to have clearance to groove on the face. You cannot simply take an OD grooving tool and use it on the face without first grinding some heel clearance if that is the only tool you have to use.

 

[Lee Yeomans]

The only information you provided it was a 7.5mm radius groove. I am assuming the depth of the face groove is also 7.5mm?

I need all of the diameters and lengths for the feature and also the radius tangent to the 7.5mm groove to help you out.

I would program this in two units. Turn the OD with a CNMG tool and then cut the face groove with your 6mm radius tool. Keep in mind, the 6mm tool will need to have clearance to groove on the face. You cannot simply take an OD grooving tool and use it on the face without first grinding some heel clearance if that is the only tool you have to use.

Hi, sorry for the delay, not been at work, I’ve done a a drawing of the detail, as not aloud to send drawing, hopefully there is the relevant info on there

 

[Philabuster]

Here's the Mazatrol program and the tool data and tool file for tool 12. You mentioned it was a 6mm radius tool so that is what I have in the Tool Data. If it is in fact a 6mm wide tool, then change the tool's radius value to 3mm.

 

[Philabuster]

On second thought, delete the 2mm chamfer from the face radius unit and machine that feature using another unit and tool.

 

[Lee Yeomans]

Here's the Mazatrol program and the tool data and tool file for tool 12. You mentioned it was a 6mm radius tool so that is what I have in the Tool Data. If it is in fact a 6mm wide tool, then change the tool's radius value to 3mm.

Awesome, thank you, I will give that a whirl when I have finished my current job, much appreciated

 

[Philabuster]

Awesome, thank you, I will give that a whirl when I have finished my current job, much appreciated

You will have to figure out the feeds and speeds though. I just helped you to create the program.

You should be able to describe the tool as a face grooving tool with a full radius.

Alternately, you can describe the tool as a General Edge tool with a 3° primary angle and a 0° secondary angle like I did. The tool path did not work for me using a grooving tool because my machine is setup in inches--not metric. The machine got confused because I told it the grooving tool was 12" wide. I basically programmed the part as if it was 185 inches in diameter in order to get you the info.