4th axis settings for part diameter

[vmax549]

Does anyone know if Tormach assigned a #var to the 4th axis part diameter DRO. It woul dbe used to set the part diameter from Gcode on program load.

(;-) TP

Similar Threads:

• Need Help!- Milling 3d part settings
• Need Help!- Condition Settings for brass diameter electrode
• Problem- Trouble Rotary Milling with CPLs on a Part's Outside Diameter
• Stock part settings and other questions
• Shaft Diameter, LeadScrew Diameter, Motor Torque?

[kstrauss]

I am not aware of a "4th axis part diameter DRO" nor even a "4th axis part diameter" in PP. Mach3 has such a kludge; depending on your application inverse time mode (G93) may be useful.

Or did you mean the diameter that can be entered on the Settings/4th axis screen for 4th axis related probing? I didn't realize that that did anything other than make probing faster.

[vmax549]

I assumed that it also set the coordinated feedrate on the rotary . EVERY modern controller has such a setting. So far PP has a terrible 4th axis toolpathing display. It displays as inside out and upside down all at the same time. The update said they worked on it and made it better but I don't see it.

Just a thought, (;-) TP

[kstrauss]

I assumed that it also set the coordinated feedrate on the rotary . EVERY modern controller has such a setting.

Perhaps but is it a part of RS-274?

[vmax549]

There has been of LOT of improvement in CNC that is not RS-274 related (;-) The last update on RS-274 that I read was at least 20 years old.

There really is not a reason to NOT have 4th axis diameter setting.

Just a thought , (;-) TP

[kstrauss]

Extensions may be good but using a manually entered diameter seems mostly useless. Most 4th axis jobs will cut below the surface of the initial cylinder so the diameter will change. How does one adjust the "diameter" if one is machining square or hex or other shapes? Generalizing "diameter" as a solution for five or more axis seems even more problematic. Have you considered using G93?

[vmax549]

Sure I use G93 "when" it is needed but when I am just doing surface machining on a cylinder why bother . 4th axis diameter comp works fine for everything up to deep carving. When you have an uneven surface you simply pick the largest diam you are working with. The machine then comps the Feedrate to match that. When you get to a low spot it just moves a touch slower. Overall it has always worked well. Fanuc has it so does Haas,Mits,Mazak and most other controllers I have used over the last 50 years.

I am more concerned over the bad 4th axis toolpath display. ON a first artical you really need to see the Backplot correctly.

(;-) TP

[kstrauss]

Agreed about the backplot. At least it is considerably less useless than in previous versions!

[vmax549]

OK I had to get Tormach to SPLAIN teh 4th axis toolpathing . You do HAVE to do teh 4th axis setup in settings. Either probe for A axis center or enter the data manually . That centerpoint defines teh center of rotation for teh toolpath display . BUT it does not set the x/y/A feedrate like Haas par34. They are working on that part.

Thank You Tormach

(;-) TP

[kstrauss]

Does the diameter defined in Settings/4th Axis Rotary currently have any effect? Can you set Z and Y centre programmatically or only by using the setup screen?

[ally-g]

I have always used G10 L2 to define my 4th axis centre in my programs and have put my normal offsets into the new settings page and have not had anything unusual happen yet.I cannot see how the settings used in the settings page would override offsets written into a program.For feed I use G93 inverse time.Nothing I do is particularly complex,spiral fluting bolts is one of the more common.

[vmax549]

This was Tormachs suggestion on the matter

" We typically recommend that you set a work offset at the A-axis center for Y and Z. If you pick a particular work offset (say G59) for your 4th axis programs, you shouldn’t need to update the center position values in every program. You would typically update the offset values only when you physically move the axis on the table, or set up a new fixture. "
-Rob

Personally I would do it from Gcode in teh preamble(safety Block) JUST to make sure it did not get missed . You could do it with G10 or possible with a set of #vars defined with teh values.

(;-) TP

[mountaindew]

wow, sounds like lots of time.
Glad I just model part in cad and setup part in cam.
Load gcode, find and zero x,y,z,a, g5? hit run and change tools until its done. Only annoying part is unwinding axis back to zero when new operation is started.
Guess cam bloatware has its advantages. Unless your doing something complex like cam lobes it takes only minutes to setup most 4th axis programs. "with experience"
That said the code is often not efficient and a single cam setting can balloon the size of the compiled g-code file with little or no real difference in results.