Can CamBam create a toolpath for a parting tool on lathe?

[dh42]

Hello

On your drawing, you assume that the Z = 0 is at the middle of the tool, but it's not the case, the 0 is at the left corner, as explained on the manual.

Lathe Tool Radius Offset    

If False, the toolpath at the center of the tool radius is output.

If True, an appropriate tool radius offset is applied. The toolpath will be offset by a negative tool radius in the lathe X axis. The direction of the Z tool radius offset is determined by the cut direction. For right hand cuts the toolpath Z will be offset by a negative tool radius. For left hand cuts, a positive tool radius Z offset is used.



In the diagram above, the red cross represents the toolpath reference point when Lathe Tool Radius Offset is set True. If False, the dot at the tool radius center will be the reference point. The reference point is sometimes referred to as the 'Imaginary' or 'Virtual' tool point.

http://www.cambam.info/doc/dw/1.0.0/cam/lathe.html

++
David

[EddyCurrent]

I think the CamBam toolpath is fine for ball nose tools.
The toolpath follows the centre of the ball, for example if a 6mm ball nose tool was used then the toolpath would be 3mm offset from the cut surface.

not as simple as that
have u ever used cambam to turn?
it is not offeset, the offset is there when the side cuts but when the front cuts then there should not be any offsets and that the complexity of it

No, if the "Lathe Tool Radius Offset" parameter in the post processor is set to "False" then the toolpath will follow the centre of the ball specifed by "tool radius",  that's what the manual says not me.

Do yourself a favour and get a ball nose tool.

[GraphicMan]

"i am afraid that is totally not correct
just think about it, the very near feature should have the tool in contact on the profile no with an offset, you will be surprised on how the real toolpath should look like for either a square or a rounded parting tool"
----------
REALLY?

I'm bowing out.  You know far more about how CamBam should work than all the folks who've been using it all these years!

Lloyd

take a look at the last capture i shared, look how different the toolpath than the profile
a simple offset does not make a toolpath
what am i missing?!

[GraphicMan]

in that case the toolpath generated is different than the post processed one?
i did not turn anything off
i have not checked a saved path yet

[GraphicMan]

the saved toolpath is nothing different than the generated one, just offset still!

[dh42]

after a small test, it appears that the toolpaths are always offseted on the CamBam display regardless of the "Lathe Tool Radius Offset" parameter in the post processor. but in the Gcode the toolpath changes

I attach a .cb file.

It is a 10mm radius rod with a sphere at the right end, tool diameter set to 1mm

CamBam always shows the toolpath with the radius offset. as on this picture.



But depending of the setting of "Lathe Tool Radius Offset" the Gcode is different.

With true:

Code: [Select]

( Tournage1 - TRUE)
M6 T0101
G18
M3 S3000
G0 Z30.0
G0 X1.5
G1 F600.0 X-0.5
G2 F800.0 X10.0 Z19.5 I0.0 K-10.5
G1 Z-0.5
G0 X50.0
G0 X50.0

With false

Code: [Select]

( Tournage2 - FALSE )
M6 T0101
G18
M3 S3000
G0 Z30.5
G0 X2.0
G1 F600.0 X0.0
G2 F800.0 X10.5 Z20.0 I0.0 K-10.5
G1 Z0.0
G0 X50.0

This picture shows the 2 different toolpaths obtained on NCplot (merged in one unique Gcode for display)



++
David

[dh42]

and the strange things is that it's when "Lathe Tool Radius Offset" = false that the toolpaths are offsetted, and they are not affected with true ... I think its reversed

++
David

[GraphicMan]

and the strange things is that it's when "Lathe Tool Radius Offset" = false that the toolpaths are offsetted, and they are not affected with true ... I think its reversed

++
David

told u man, it is truly messed up
why nobody wants to believe?!!
btw make something similar to wut i have initially shared to see that it is still just offset even on the gcode, try it

[dh42]

Yes but as said in the manual 

Note: The lathe code is new to version 0.9.8 and is still undergoing testing and development.
Treat any lathe gcode with caution and run simulations or air cuts before machining.

and of course, the Lathe plugin is the same in V1.0 ..

++
David

[GraphicMan]

Yes but as said in the manual 

Note: The lathe code is new to version 0.9.8 and is still undergoing testing and development.
Treat any lathe gcode with caution and run simulations or air cuts before machining.

and of course, the Lathe plugin is the same in V1.0 ..

++
David

yes i was even using ver 1 !!
this plugin does not make any sense! i have no idea why the mods where arguing then!
thank u very much for taking the time to verify the issue i was asking for

[dh42]

I don't have CNC lathe, so I can't know, but it seems that some peoples here use it and that they can obtain what they want ...

++
David

[lloydsp]

David,
From what I've seen, he's still thinking "square-end tool", and the plugin is designed for a semi-circular tool tip.  But that doesn't seem to register.

Eh... It's not worth my time to tell him others are using it with success.  He won't believe it.

Lloyd

[GraphicMan]

David,
From what I've seen, he's still thinking "square-end tool", and the plugin is designed for a semi-circular tool tip.  But that doesn't seem to register.

Eh... It's not worth my time to tell him others are using it with success.  He won't believe it.

Lloyd

r u really still arguing about it?
have u used it urself?
do u turn?
i told you it does not matter if it is square or round
even with a round tool it does not work, just give urself the time to imagine it
or look back at the drawing i shared!

[dh42]

he's still thinking "square-end tool"

Like a groowing tool ?

++
David

[dave benson]

Hi GraphicMan

I've been using a cnc lathe (Artificial Intelligent tool changer but no bar feeder) for about 10 years
now,(the last three with the tool changer) I did look into CB for working with the lathe, and discovered
that it was not able to do any  of the normal operations usually associated with making a component.(even a fairly simple one)
So I had to look around for something else that would do the job.
I found two pieces of software that I've settled on.

1... Ezilathe  free from cnczone. 
You can do the cad work in CB and import it with Ezilathe or just draw it in Ezilathe
2...Fusion360

For simple (once jobs only) I just use the wizards in Mach3, threading,boring,facing and for parting off I use the OD groove wizard.
For little more complex work Ezilathe, and for the most complex (involving many tool changes) I use fusion.

Dave