Bolt hole circle and circular interpulation probs

[Doug*]

Just started woking at a new place and they would like me to program their Okuma MC-4VA CNC vertical mill. Can anyone help me with a sample program for both circular interpulation and bolt hole circle? For example, a 4" circle starting at 45 degrees with 8 holes drilling though 1/2" steel (for the BHC) and maybe a 2" circle using a 1/2" endmill. I can then take these examples and modify them to each job that comes up. The control on the machine is an Okuma OSP5000M-G.

Thanks!

[broby]

Hi Doug,
How much programming experience do you have?
It would be much better learning how to do this in the long run, rather than having us do your work for you all the time.
I assume you mean in your request that you want a program to drill 8 holes on a 4" PCD with the holes equally spaced and the first hole is at 45 degrees?
Also you require a program to mill a circle?
Do you understand the use of G2 or G3 and the associated vectors I,J & K?
Okuma also has a very easy to use BHC command that allows easy programming of a Bolt Hole Circle.
for example...
Assuming Z0 is the TOP Surface, Speed is set, Coolant is as required.
Co-Ordinate system is set...
N100 G71 Z0.1
N102 NCYCL G81 X0 Y0 Z-0.6 R0.05 Fxxxx M53
N104 BHC X0 Y0 I2.0 J45 K8
N106 G0 Z0.1
etc...

Where I is the Radius of the PCD
J is the starting angle with 0 degrees being at 3 O'Clock
K is the number of points, K-8 would do the holes CCW rather than CW direction.

Hope this gets you started.
Regards
Brian.

PS good luck with the job.
Come back often and ask plenty of questions, just do not ask us to do your job entirely for you.

[Doug*]

I hate to bug you again but I'm still having problems......First let me give you the first 12 lines of my program:
N10 G90 G01 G94
N20 G00
N30 G56 M06 T1
N40 M01
N50 M03 S500
N60 M08
N70 G90 X0 Y0 Z.5
N80 G02
N90 G71 Z0.1
N100 NCYCL G81 X0 Y0 Z-0.6 R0.05 F5 M53
N110 BHC X0 Y0 I2.0 J45 K8
N120 G00 Z0.1

When it comes to line N100, it causes alarm 429 ALARM B Unusable: direct of left side 3602. If I delete the NCYCL part of the line, it will cause an alarm on line 110 that says: 461 ALARM B Data Word: spec code 11. When I remove both the NCYCL and BHC portions of lines N100 & N110, It doesn't alarm out but will only drill one hole. I should probably mention that the machine control, when read from the edit date page, reads 4-1-1984. Would the age of the machine have anything to do with it not understanding the NCYCL and/or BHC commands?----Or is it my lack of experience has caused an error or missing info further up towards the beginning of the program?

Thanks again for your help,
Doug

[littlerob]

I think (and I know what they will say about that) you need to remove line # 80 (G02), you shouldn't be using a clockwise arc command before your drill cycle.

The I, J and K commands Brian was explaining are a little different with the BHC than circular interpolation say with an end mill. Radius, angle to begin at, and repetitions.

I=Rabius (4" circle 2" radius), J=angle (complete circle 8 holes, 360/8=J45), K=repetitions (8 holes K8). But that G2 is what is giving you alarms I'm willing to bet on it AU$.

Robert

Like Brian said "come back with lots of questions", it gives us something to do.

[Doug*]

I appreciate your input and idea but I only added line 80 (G02) out of desperation. I've tried it without that line again and still get the same alarms. It has really been tough to figure this one out.

Doug

[broby]

I hate to bug you again but I'm still having problems......First let me give you the first 12 lines of my program:
N10 G90 G01 G94
N20 G00
N30 G56 M06 T1
N40 M01
N50 M03 S500
N60 M08
N70 G90 X0 Y0 Z.5
N80 G02
N90 G71 Z0.1
N100 NCYCL G81 X0 Y0 Z-0.6 R0.05 F5 M53
N110 BHC X0 Y0 I2.0 J45 K8
N120 G00 Z0.1

When it comes to line N100, it causes alarm 429 ALARM B Unusable: direct of left side 3602. If I delete the NCYCL part of the line, it will cause an alarm on line 110 that says: 461 ALARM B Data Word: spec code 11. When I remove both the NCYCL and BHC portions of lines N100 & N110, It doesn't alarm out but will only drill one hole. I should probably mention that the machine control, when read from the edit date page, reads 4-1-1984. Would the age of the machine have anything to do with it not understanding the NCYCL and/or BHC commands?----Or is it my lack of experience has caused an error or missing info further up towards the beginning of the program?

Thanks again for your help,
Doug

Well don't I feel the right doofus!
The command to ignore the drilling cycle at the selected posn on Line N100 should be NCYL not NCYCL.
You definitely do not use the G2 on line N80.

your program should look like:
N10 G90 G01 G94
N20 G00
N30 M06 T1
N40 M01
N50 M03 S500
N60 M08
N70 G56 HA Z40
N80 G90 X0 Y0 Z.5
N90 G71 Z0.1
N100 NCYL G81 X0 Y0 Z-0.6 R0.05 F5 M53
N110 BHC X0 Y0 I2.0 J45 K8
N120 G00 Z0.1
etc...

Note the addition of the HA command on Line N70, rather than on the tool change line. While your method would probably work (I have never programmed tool length offset that way) I preferr to use the command AFTER the tool is into the machine.
The HA command tells the machine to use the tool length offset for the ACTIVE tool and move to Z40 turning on Tool Length Compensation as you go.
The more common method is to specify the tool number in use when calling tool length comp, i.e. use G56 H1 (Tool 1 length).
I use the command HA all the time for two reasons:
1. Constantly changing tool locations in the machine mean less program editing.
2. One of the machines uses Tool Groups and with potential multiple tools in a group, I have no option but to use Active tool programming.
Tools can be programmed using HA, HB & HC for three length offsets and DA, DB and DC for three different Tool Radius offsets. This comes in very handy when programming chamfering tools... I use HA/DA for the Length/Radius at the end of the tool, then HB/DB for the point at the end of the front taper, then HC/DC for the "Back" edge of the taper (see attached image) but I digress... you can figure that one out later.

I suspect that MAYBE you do not have the option for using BHC on your machine...? That could be the reason for the Alarm "461 ALARM B Data Word: spec code 11" (which came up after removing the NCYCL?).
if that is the case then you have no choice but to manually program each hole position.
i.e.
N10 G90 G01 G94
N20 G00
N30 M06 T1
N40 M01
N50 M03 S500
N60 M08
N70 G56 HA Z40
N80 G90 X1.4142 Y1.4142 Z.5
N90 G71 Z0.1
N100 G81 Z-0.6 R0.05 F5 M53
N110 X0 Y2
N120 X-1.4142 Y1.4142
N130 X-2.0 Y0
N140 X-1.4142 Y-1.4142
N150 X0 Y-2.0
N160 X1.4142 Y-1.4142
N170 X2.0 Y0
N180 G00 Z0.1
etc...

Notice also that I am using the Rapid Command G00 to cancel the drilling cycle... rather than G80. G80 will stop the spindle at the end of the drilling cycle so if you use G80 and want to use the current tool for more work, the spindle will be stopped... using the G00 command allows the spindle to keep going and cancels the drilling cycle.

Hope this helps,
Brian.

[underthetire]

Call Okuma or your local distributor and see if you can get the old classroom workbook they handed out. I used to give them away when I taught class on those many years ago. It has plenty of examples of what you need.

[DIFF OVER]

I thought BHC is only if you have IMAP.

[broby]

I thought BHC is only if you have IMAP.

Nup!
I have this available on our old MC600 (OSP5020M) ~15years old, and this machine does not have the IMAP function.

Mind you, Doug does state that his control is OSP5000M-G not the 5020...
This could be the difference.
Cheers
Brian

[Superman]

N80 G90 X0 Y0 Z.5
N90 G71 Z0.1
N100 NCYL G81 X0 Y0 Z-0.6 R0.05 F5 M53
N110 BHC X0 Y0 I2.0 J45 K8

I think the double up of the centre of the cycle is creating the problem
The centre point defaults to the tool's position if omitted, but to make it safe, I would have the position in the cycle call ( in blue )

N80 G90 X0 Y0 Z.5
N90 G71 Z0.1
N100 NCYL G81 Z-0.6 R0.05 F5 M53 ( actual pattern )
N110 BHC X0 Y0 I2.0 J45 K8 ( pattern done here,and in this way )

[broby]

I think the double up of the centre of the cycle is creating the problem
The centre point defaults to the tool's position if omitted, but to make it safe, I would have the position in the cycle call ( in blue )

N80 G90 X0 Y0 Z.5
N90 G71 Z0.1
N100 NCYCL G81 Z-0.6 R0.05 F5 M53 ( actual pattern )
N110 BHC X0 Y0 I2.0 J45 K8 ( pattern done here,and in this way )

Was wondering if you were going to stick your 2c worth in some time or another Steve
Actually, you are incorrect with your suggestion, the whole point of the NCYL command (NOT NCYCL) is to tell the machine that No CYcLe is to be done at this line position. i.e. setup the drilling cycle (in this case) and do no machining... then using the cycle defined, do it at the points designated by the BHC pattern (or point by point pattern).
The fact that the machine is bringing up an Spec Code alarm tells me that the machine does understand the BHC command, just that the machine does NOT have that Specification.
i.e. it is an optional extra not installed on Doug's mill
Brian.

[Superman]

Ok, I pasted the CYCL from lower down, so my previous post is now good
( I wonder where that started ??? )

We have the MC-4VA OSP5000-M

Canned cycles are standard I thought, book doesn't say it is an option
we don't have the 3-axis circular interpolation, so no ramping on circles