Hi all!
Is it possible to produce the way outlined in the picture? I would like to deal the radius R10 archedly with the axis Z, from Z+0 to Z+10. According to the Control Software Features of the Heidenhain Manual ist must work:
"3. circular interpolation on any two axes, i.e. XY, XZ or YZ, whit linear interpolation on the third axis"
How does this work?
Regards
Enny
Triac VMC Toolpath
Moderators: Martin, Steve, Mr Magoo
Triac VMC Toolpath
- Attachments
-
- pfad.GIF (3 KiB) Viewed 6354 times
-
davidimurray
- CNC Expert
- Posts: 194
- Joined: Thu 24 Aug , 2006 9:45 am
I'm not familiar with that particular machine, but you will want to interpolate an arc in the YZ plane, then an offset in X, YZ Arc, x offset etc.
To do this you will need to use a ballnose cutter. The finish will be a series of small ripples - the smaller the X offset the smaller the ripples.
If the profile is half round and not too large then you could simply get hold of a ballnose cutter of the right size.
Cheers
Dave
To do this you will need to use a ballnose cutter. The finish will be a series of small ripples - the smaller the X offset the smaller the ripples.
If the profile is half round and not too large then you could simply get hold of a ballnose cutter of the right size.
Cheers
Dave
-
Denford Admin
- Site Admin
- Posts: 3634
- Joined: Fri 10 Feb , 2006 12:40 pm
- Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then. - Location: Sunny Brighouse
- Contact:
I think you'll find the linear interpolation on the third axis is to create a Helical movement.XY, XZ or YZ, whit linear interpolation on the third axis
You define the arc as normal, say 180 degrees in the XZ plane
Then the third value (Y) will interpolate the given amount while the arc is in progressing round (0-180 deg).
I don't think this is what you wanted ? Unless you create a long series of helical arcs (the tool path would then look like a thread)
I also think you will have to use a ball nose cutter
Hello!
Thank you for the answers.
Unfortunately, I have expressed myself a little wrongly. It is not all about for me which strategy I can employ or which cutter. I "simply" need a way to enter the machine the coordinates.
It already starts, the small machine is not ready to countersink a circle. The following inputs do not cause movement of the machine, the simulation be correctly carried out.
CC X+0 Y+0
CP PA+360 DR+ R F M
If I replace PA by the value +359.9, it drives along the path correctly!?
To the real problem back!
Dave describes the approach completely correctly. However, I have no idea how I get this in a program.
In my opinion this should approximately look that way:
BEGIN PGM 1 MM
:
X+45 Y+0 R F M
Z-10 R F M
CC X+45 Z+0
C Y+45 Z+0 R F M
:
The input of CC X+0 Z+0 causes the disappearance of the line in the editor.
The input of C X+0 Z+0 DR+R F M causes the error message " Invalid Arc end point ".
The input of CT X+0 Z+0 R F M causes a movement which corresponds to CP PA+180.
I have tried it also with TOOl CALL 1 X S4000, tried also with Y. No successes!
I could hopefully make clear where my problems lie. Perhaps this can explain somebody to me. Best with a simple Proramm as an example.
It is the original Heidenhain Contol V1.86.
Best wishes
Enny
Thank you for the answers.
Unfortunately, I have expressed myself a little wrongly. It is not all about for me which strategy I can employ or which cutter. I "simply" need a way to enter the machine the coordinates.
It already starts, the small machine is not ready to countersink a circle. The following inputs do not cause movement of the machine, the simulation be correctly carried out.
CC X+0 Y+0
CP PA+360 DR+ R F M
If I replace PA by the value +359.9, it drives along the path correctly!?
To the real problem back!
Dave describes the approach completely correctly. However, I have no idea how I get this in a program.
In my opinion this should approximately look that way:
BEGIN PGM 1 MM
:
X+45 Y+0 R F M
Z-10 R F M
CC X+45 Z+0
C Y+45 Z+0 R F M
:
The input of CC X+0 Z+0 causes the disappearance of the line in the editor.
The input of C X+0 Z+0 DR+R F M causes the error message " Invalid Arc end point ".
The input of CT X+0 Z+0 R F M causes a movement which corresponds to CP PA+180.
I have tried it also with TOOl CALL 1 X S4000, tried also with Y. No successes!
I could hopefully make clear where my problems lie. Perhaps this can explain somebody to me. Best with a simple Proramm as an example.
It is the original Heidenhain Contol V1.86.
Best wishes
Enny
Hi Enny
I think your machine only supports arcs in the XY plane (some earlier versions of the firmware inside the machine did not support plane switching - ie arcs in the XZ and YZ planes)
If the machine did support it then the format of the program would be similar to...
TOOL CALL 1 X (tool comp is in the X plane, arcs in YZ plane)
L X0 Y20 Z0 (linear move to Y+20)
CC Y0 Z0 (CC at Y0 Z0)
C CW Y-20 R20 (CW move to Y-20, rad of 20)
The last ver of the Heiden sware for Triac was v2.119 (September 1998). You could try this but I think the problem is in the machines firmware so you can not (easily) upgrade without hardware changes.
An alternative option is to use Q parameter programming. This lets you write a CNC prog using variables and math functions.
QDEF Q1 = 10 (Q1=10)
QDEF Q2 = 20 (Q2=20)
L XQ1 YQ2 (Linear to X10 Y20)
You have functions like SIN, COS as well as condition jumps like IF Q1<50 GOTO LABEL 1 so you could write a loop to produce the arc as lots of small linears. Maybe not the ideal solution but could help?
I think your machine only supports arcs in the XY plane (some earlier versions of the firmware inside the machine did not support plane switching - ie arcs in the XZ and YZ planes)
If the machine did support it then the format of the program would be similar to...
TOOL CALL 1 X (tool comp is in the X plane, arcs in YZ plane)
L X0 Y20 Z0 (linear move to Y+20)
CC Y0 Z0 (CC at Y0 Z0)
C CW Y-20 R20 (CW move to Y-20, rad of 20)
The last ver of the Heiden sware for Triac was v2.119 (September 1998). You could try this but I think the problem is in the machines firmware so you can not (easily) upgrade without hardware changes.
An alternative option is to use Q parameter programming. This lets you write a CNC prog using variables and math functions.
QDEF Q1 = 10 (Q1=10)
QDEF Q2 = 20 (Q2=20)
L XQ1 YQ2 (Linear to X10 Y20)
You have functions like SIN, COS as well as condition jumps like IF Q1<50 GOTO LABEL 1 so you could write a loop to produce the arc as lots of small linears. Maybe not the ideal solution but could help?
Hello Mr. Magoo!
Thank you for the answer. Unfortunately, it is not what I would have enjoyed reading.
Since the possibility is described in the manual I thought I am too stupid to use it.
I know the possibilities of the parameter programming and find these very useful.
But what uses this to me if the simple things not functioning like them should?
E.g. what do you say to the CP PA+360 DR+ problem? Circles with radii over 140 mm paralyze the control completely. I do not use the radius correction any more. It leads to completely strange outputs of the control.
I would like to use the version 2,119 loving. Unfortunately, I need another EPROM to this! And possibly still more! Please, cannot somebody get these EPROM to me?? Please, please!
Best wishes
Enny
Thank you for the answer. Unfortunately, it is not what I would have enjoyed reading.
Since the possibility is described in the manual I thought I am too stupid to use it.
I know the possibilities of the parameter programming and find these very useful.
But what uses this to me if the simple things not functioning like them should?
E.g. what do you say to the CP PA+360 DR+ problem? Circles with radii over 140 mm paralyze the control completely. I do not use the radius correction any more. It leads to completely strange outputs of the control.
I would like to use the version 2,119 loving. Unfortunately, I need another EPROM to this! And possibly still more! Please, cannot somebody get these EPROM to me?? Please, please!
Best wishes
Enny
Enny...
I think your only option is to upgrade your existing motion control card inside the machine with a "NextStep" card (you will need to ask Denford about this).
Advantage: Gives you arcs in the XZ and YZ plane
Disadvantage (for you): Can only use VR Milling software which is programmed using FANUC G Codes (not Heidenhain dialog format).
I think your only option is to upgrade your existing motion control card inside the machine with a "NextStep" card (you will need to ask Denford about this).
Advantage: Gives you arcs in the XZ and YZ plane
Disadvantage (for you): Can only use VR Milling software which is programmed using FANUC G Codes (not Heidenhain dialog format).