Lathe cutter comp and FRONT/BACK tool table entrie

More
17 Mar 2015 07:41 - 17 Mar 2015 07:42 #56906 by drogge
I'm trying to machine a ballpin and am having trouble with cutter compensation. Everything looks fine on the end of the ball closest to the tailstock but the compensation seems backwards when I go past 90 degrees, the tool path is moved away from the part at the 45 instead of closer. Angles also get weird. The cutter gets closer to the part on angles that increase in size as they approach the spindle but moves away from angles that get smaller. I've attached a copy of the gcode and an image of the path generated by linuxcnc (version 2.6.5). The red path is without cutter comp and the white path is with G42 cutter comp.

For what it's worth the machine has a back tool post if that makes any difference. Messing around with the tool table got me to wondering what the FRONT and BACK entries are used for by linuxcnc. I searched linuxcnc.org but couldn't find any info on what effect they have.

Thanks for any info,
Drew
Attachments:
Last edit: 17 Mar 2015 07:42 by drogge.

Please Log in or Create an account to join the conversation.

More
17 Mar 2015 09:06 #56909 by joekline9
I don't think front and back angles are used for tool path.
Linuxcnc uses the control point and tool radius. The red line is the path of the control point.
Orientation determines the control point. (See manual for lathe)

I hope this helps you.

Please Log in or Create an account to join the conversation.

More
17 Mar 2015 17:24 #56930 by emcPT
Hello,

I use linuxcnc on lathes. If you are used to the tool orientation of all other machines, and if you use the back tool post, on linuxcnc for a reason that I do not know (I think it was a mistake at the implementation, and never went corrected), the orientation is swapped.

For example if your tool have orientation 2 on a Fanuc machine, in linuxCNC it have 3.

If you look for a post that I did before, I made a patch to correct this, but I think that nobody had interest in it and never was placed on the source code.

Please Log in or Create an account to join the conversation.

More
17 Mar 2015 20:04 #56941 by andypugh

I use linuxcnc on lathes. If you are used to the tool orientation of all other machines, and if you use the back tool post, on linuxcnc for a reason that I do not know (I think it was a mistake at the implementation, and never went corrected), the orientation is swapped.


Indeed. The LinuxCNC tool orientations were based on a diagram from an existing lathe manufacturer, but it wasn't noticed for several years that the original diagram was for a back-toolpost lathe. This means that the LinuxCNC tool orientations are not the same as the Okuma / Fanuc ones. This is unfortunate but the post-processors and existing code now follows the "new standard" and so it is not an easy thing to swap the orientations now.

Please Log in or Create an account to join the conversation.

More
17 Mar 2015 20:08 #56942 by andypugh

The cutter gets closer to the part on angles that increase in size as they approach the spindle but moves away from angles that get smaller.


This might not be wrong, the red line shows the "controlled point" and that is outside the tool tip for most lathe tool orientations.

Which Tool orientation number are you using? Bear in mind that the LinuxCNC diagram shows a front-tool lathe so you have to flip it for back-toolpost.

Please Log in or Create an account to join the conversation.

More
18 Mar 2015 01:25 - 18 Mar 2015 01:31 #56956 by drogge
I'm using tool orientation 2. I found this document that shows the difference between front tool post, back tool post and Fanuc.

I was thinking about this last night as I was lying in bed and I think the problem is that I'm assuming that the tool radius is concentric to the control point and that's only the case with a number 0 tool radius. I'm just going to cut the part and see what happens.

Thanks for all the help everyone.

Drew
Last edit: 18 Mar 2015 01:31 by drogge.

Please Log in or Create an account to join the conversation.

More
18 Mar 2015 02:23 #56960 by andypugh

I think the problem is that I'm assuming that the tool radius is concentric to the control point and that's only the case with a number 0 tool radius.


Exactly. With Orientation 2 the controlled point is outside the tip.

If you make sure that with compensation OFF the tip is turning to exact diameter and length, then with Orientation 2 and compensation on you should get a true hemisphere on the right-hand face.
It isn't at all clear to me what the left-side faces will do. Cutter comp only considers the tool as a disc. (at best) and has no idea about front and back angles.

if you want to accurately profile both sides then you probably need to use two tools. Or an orientation 0 tool.

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.941 seconds
Powered by Kunena Forum