CamBam

Support => Lathes and Turning => Topic started by: GraphicMan on May 25, 2021, 15:32:26 pm

Title: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 15:32:26 pm
Hello

As far as i have read cambam can create toolpaths for simple profiling on a lathe
but how? i could not find how to specify the tool geometry being used
i will be using a 2mm wide square parting tool
attached the profile need to be cut
i know that the back of the ball cant be made exactly as desired, it will be fine with a straight line of 2mm after the ball
thanks
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: EddyCurrent on May 25, 2021, 15:47:50 pm
From the manual;

"The file lathe-test.cb in the CamBam samples folder demonstrates the new lathe operation.

In this initial lathe release there are a number of limitations:

    Only profiling operations are currently supported. No facing, boring or threading support yet.
    Apart from the tool radius, there is no mechanism to define a lathe tool shape. The part should be drawn to allow for the cutter size and shape."

Once CamBam is opened click on "Help" to bring up the manual, there is a section on using the lathe function and also sample files in, "Tools->Browse System Folder->Samples"
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 16:15:40 pm
From the manual;

"The file lathe-test.cb in the CamBam samples folder demonstrates the new lathe operation.

In this initial lathe release there are a number of limitations:

    Only profiling operations are currently supported. No facing, boring or threading support yet.
    Apart from the tool radius, there is no mechanism to define a lathe tool shape. The part should be drawn to allow for the cutter size and shape."

Once CamBam is opened click on "Help" to bring up the manual, there is a section on using the lathe function and also sample files in, "Tools->Browse System Folder->Samples"

thanks for your prompt respond
i have checked all that, the problem is that cambam seems like it is using turning as round tool only
there is no other tool geometry that it can understand?
we need someone who have actually used its turning capability
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: EddyCurrent on May 25, 2021, 16:21:35 pm
Even without CamBam, just using a manual lathe, it is highly unlikely that anyone would choose to machine your part with a 2mm wide square parting tool.
CamBam uses the equivalent of a ball nose tool in standard cnc mode.

It may be possible to specify a tool radius of zero, give it a try and see what the toolpaths look like.
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 16:34:53 pm
Even without CamBam, just using a manual lathe, it is highly unlikely that anyone would choose to machine your part with a 2mm wide square parting tool.
CamBam uses the equivalent of a ball nose tool in standard cnc mode.

It may be possible to specify a tool radius of zero, give it a try and see what the toolpaths look like.
yes indeed i do a lot with a 2mm wide parting tool
if u specify a very small radius for the tool it will generate a toolpath that is way off the desired one
think about it, the toolpath needed should respect both sides of the tool
i think cambam will not do that, so sad
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: lloydsp on May 25, 2021, 17:23:44 pm
Try an infinitely-large (well.. very large) radius.  The 'radius' of a flat-nosed tool is infinite.

But really -- a flat-faced parting tool as a profiling tool?  Really?

Lloyd
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: Bubba on May 25, 2021, 17:28:59 pm
But really -- a flat-faced parting tool as a profiling tool?  Really?
***************************
Exactly what I was wondering...
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 18:19:25 pm
even for a round parting tool it does seem that cambam is doing any real toolpath
it is just offsetting the original profile?!!
all the tests i have tried is just offseting !

Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: lloydsp on May 25, 2021, 19:04:26 pm
Graphicman,

That might be all it needs to do to cut a profile with a radiussed tool.

Lots of people use it, and it seems to work to their pleasure.

Lloyd
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 19:22:26 pm
Graphicman,

That might be all it needs to do to cut a profile with a radiussed tool.

Lots of people use it, and it seems to work to their pleasure.

Lloyd
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: EddyCurrent on May 25, 2021, 19:28:43 pm
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.
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 19:29:06 pm
this is how the toolpath should look like in red
the rectangle represents the tool profile
i dont think cambam can generate this and i dont understand how people are using it (if any are)
now imagine the tool profile have a radius, not much will change, it will never be like what cambam generates
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: EddyCurrent on May 25, 2021, 19:31:58 pm
From the manual;


"Post Processor

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."

So for me answer would be to use a ball nose cutter and set the option to "False" in the post processor.
Why limit yourself to a 2mm square tool when you can get a ball nose tool and the problem is solved ?
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 19:33:03 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: lloydsp on May 25, 2021, 19:34:01 pm
"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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 19:35:32 pm
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.

(http://www.cambam.info/doc/dw/1.0.0/images/cam/tool-radius-offset.png)

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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: EddyCurrent on May 25, 2021, 19:37:20 pm
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.
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 19:41:43 pm
"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?!
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 19:45:10 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 20:08:05 pm
the saved toolpath is nothing different than the generated one, just offset still!
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 20:42:15 pm
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.

(https://i41.servimg.com/u/f41/14/07/22/66/sans_141.jpg) (https://servimg.com/view/14072266/5154)

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)

(https://i41.servimg.com/u/f41/14/07/22/66/sans_142.jpg) (https://servimg.com/view/14072266/5155)

++
David



Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 20:45:24 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 21:01:59 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 22:06:44 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 22:13:56 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 22:19:16 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: lloydsp on May 25, 2021, 23:22:17 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 23:46:46 pm
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!
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dh42 on May 25, 2021, 23:51:46 pm
Quote
he's still thinking "square-end tool"

Like a groowing tool ?

++
David
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: dave benson on May 25, 2021, 23:53:25 pm
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
Title: Re: Can CamBam create a toolpath for a parting tool on lathe?
Post by: GraphicMan on May 25, 2021, 23:59:56 pm
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

tell them!
hello lloyd? so i am still wrong? we are all wrong ? i even asked a close american friend of 50+ experience he told me it does not work!

thank you v much Dave i will defiantly check Ezilathe