[Gregore]

I would like to know how the software handles tool offsets for a machine configuration with the spindle mounted on the "B" axis (vs the workpiece sitting on both rotary axis). *Are the tool length & pivot geometry entered into MadCam before generating a toolpath so that madcam computes the offsets, or does it output the tool center location and vector orientation and use the CNC control for calculating the adjusted XYZAB values to adjust for the tool geometery (or does it operate both ways).

In general, if there is a tutorial on how tool offsets are handled that would be great.

Thanks

Gregore

[svenakela]

Sorry, but I'm not following you. Why should the CAM program keep track of the tool offset? That's up to the CNC controller. If you sharpen or change the tool, are you going to post process again to get a new offset?..

[Gregore]

I understand that every tool will have a different offset , and that the numbers can be stored in the software.

I will try to rephrase the question

if the spindle has the the 5th axis (I think madcam refers to this as head / table 5th axis) then the end of the spindle is swinging an arc from the center of a rotary drive point plus the length of the tool. or when the spindle is pointing straight down it knows where it is but when it rotates to any degree away from 90 to the table the software needs to know where the end of the spindle is plus any chosen tool length.


does madcam have a place to put this number

I hope I am being more clear , my machinist friend phrased the first question maybe my newbie phrasing will make more sense.

[svenakela]

I understand that every tool will have a different offset , and that the numbers can be stored in the software.

I will try to rephrase the question

if the spindle has the the 5th axis (I think madcam refers to this as head / table 5th axis) then the end of the spindle is swinging an arc from the center of a rotary drive point plus the length of the tool. or when the spindle is pointing straight down it knows where it is but when it rotates to any degree away from 90 to the table the software needs to know where the end of the spindle is plus any chosen tool length.


does madcam have a place to put this number

I hope I am being more clear , my machinist friend phrased the first question maybe my newbie phrasing will make more sense.

No, because you are mixing up the toolpath angular and linear movements with the the trigonometry of the machine (the trajectory control). It is not up to the CAM software in any aspect to tell the CNC machine (i.e. the CNC controller) about its own geometry. The post processed toolpath - the gcode - tells the controller how the tip of the cutter should be angled or moved. If a fifth axis is 2 mm long or 1 m, that's up to the CNC software to handle.
A CAM software needs some information about the machine that is going to be used to make correct toolpaths (like in your example the head is moving, not the work piece). It also needs information about the cutter and tool holder to avoid collisions etc. Still, the outcome is a long story telling the machine how to step by step move the tip of the cutter. Like in your example the story will not be "stand still and rotate the head!", it will be "Move the tip of the cutter from where we are now to one mm to the left, up half a mm and angle it 0.41 degrees".

EDIT: With that said, let me rephrase a quote from your first post:
It does output the tool center location and vector orientation and use the CNC control for calculating the adjusted XYZAB values to adjust for the tool geometry.
That's what a CAM program do.

[JOM]

It is possible to choose if the machine controller or if madCAM should handle the TCP (Tool Center Point Control). This can be defined in the post processor. Below are two examples of post processors.

1) TCP handled by the controller.
:
:
*FIRST_MOVE*
M129 <== TCP Off.
L"b" F"feed"
M128 <== TCP On.
L "x" "y" F"feed"
L "z" "a" F"feed"
*END_SECTION*
*RAPID*
L "x" "y" "z" "a" "b" FMAX
*END_SECTION*
*RAPID_APPROACH*
L "x" "y" "z" "a" "b" FMAX
*END_SECTION*
:
:

2) TCP handled by madCAM.
:
:
*TOOLPATH_OUTPUT*
TRANSFORM <== Tells madCAM to calculate pivot compensation.
*AXIS_OFFSET*
322 <== Set the distance from pivot center to the chuck.
*TOOL_LENGTH_OFFSET*
YES <== Tells madCAM to also use the saved toolength.
*FIRST_MOVE*
N"lnbr" G1 "b" F"feed"
N"lnbr" G1 "x" "y"
N"lnbr" "a"
N"lnbr" "z"
*END_SECTION*
*RAPID*
N"lnbr" G1 "x" "y" "z" "a" "b" F10000
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" G1 "x" "y" "z" "a" "b" F10000
*END_SECTION*
:
:

Thanks,

Joakim

[Gregore]

which controllers are currently being used well with your 5th axis , which ones are the easiest to set up to perform these inverse kinematic calculations on the fly.

[Dan B]

We use Heidenhain controllers.

[svenakela]

It is possible to choose if the machine controller or if madCAM should handle the TCP (Tool Center Point Control). This can be defined in the post processor. Below are two examples of post processors.

1) TCP handled by the controller.
* snip *

2) TCP handled by madCAM.
* snip *

Thanks,

Joakim

Why on earth would one like to hard code the tool offset? Like the second example, yes it is possible, but it only emphasizes my first question; Why should the CAM program handle the tool offset?

[JOM]

There is a whole bunch of different types of 5-axis control system that is currently successfully used with madCAM. We use madCAM every day with our DMG 60 monoblock for mold making. madCAM can handle TCP calculations for any kind of machine controler. The commands are the same in the post processor regardless of the controller.

It should be mentioned, and I myself would prefer to let the control system handle the TCP calculations if possible, as this also in most cases includes the controll of feed rates at the tool tip.

Below are some video links.

Videos with TCP in the controller:
Simultaneous 5 axis milling | Flickr - Photo Sharing!
Mold Milling with 5 Axis | Flickr - Photo Sharing!

Video with TCP by madCAM:
madCAM 5Xtra - 5 axis Simultaneous Milling - YouTube

/Joakim

[Gregore]

Why on earth would one like to hard code the tool offset? Like the second example, yes it is possible, but it only emphasizes my first question; Why should the CAM program handle the tool offset?

Now that I have learned a little more about cnc mills I feel I can give a answer to this question at least from what I like and need.

First reason to have the cam handle the calculations is my friend is building my machine and to have him spend time to set it up so the controllers handle the offsets and calculation will cost money and I already bought software that can handle this.

Second , I will be cutting one offs in wax mostly so tool sharpening or breakage is a very rare issue for me at least. Also i will be running just a few parts per week and only on 1 machine. I can understand how not having to repost could save time and money in a big company with lots of machines and lots of cutting where a broken tool is easier handled with calculations in the controller. I also do not need to compensate for tool wear on multi parts.

So for me to have to do a few re-posts a year for issues that come up due to tool problems is not that big of a deal.

Wait and see how many re-posts I have to do as a newbie because I have made just plain bad choices in my tool pathing aprroch to the part in the cam software.

Gregore

[svenakela]

Lets say you make a mistake and crunch the cutter into the table or a fixture. You need to make sure your new tool is setup exactly like the broken one. Can you do that?
Both Mach and LinuxCNC which most "home made" machines uses nowadays handles offsets. As a bonus, LinuxCNC is free and MadCAM has a working post processor for LxCNC (and Mach).

/S

[Gregore]

From my perspective as a beginner I would just put another 2 dollar piece of wax in and a new tool and go again. but that is because I am not a machinist and my machine will only be running for a few hrs per week . If the machine had parts waiting to go on it. Then the most effecient way to run would be doing it all in the controller. I aslo think as a beginner there is more room for mistakes when I need to handle all the numbers rather than the cam .

[svenakela]

From my perspective as a beginner I would just put another 2 dollar piece of wax in and a new tool and go again. but that is because I am not a machinist and my machine will only be running for a few hrs per week . If the machine had parts waiting to go on it. Then the most effecient way to run would be doing it all in the controller. I aslo think as a beginner there is more room for mistakes when I need to handle all the numbers rather than the cam .

You don't see my point. Can you guarantee that the cutter will be set at exactly equal length compared to the broken one? I doubt that

[Gregore]

I do see your point, and it certainly is the correct way to do things in the milling industry . But I do not think it would be time effective to line up a cutter with a .1mm ball end back up to the same spot on the work. It seems to me that it would be better to just start over. But then again maybe by the time I have as much milling under my belt as you and many of the other members here that have the real world experience to answer our questions so accurately time after time.... I may have an opinion closer to yours.