B axis machining

[mirek1017]

Hello all!!!

 

I have same part for cuts teeth  on my HMC  .I am set up part on center of the table  and use simple 2d cut ,and I am rotate this contour 30 times .I want to get  position and B axis position ,but my post generate something like that 

 

 

T1 M6

G0 G90 G54 X-1.855 Y-12.448 B0.S1286 M3G43 H1 Z10.0681G1 Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G55 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G56 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G57 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G58 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G59 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G54.1 P1 X-1.855 Y-12.448 Z10.0681 B0.Z9.6915 F50.Y-10.648 F30.Y-4.602Y-2.802G54.1 P2 X-1.855 Y-12.448 Z10.0681 B0.

Haw  I can get  all the time G54  offset and only different  B axis ???

 

haw I can get this write????

 

 

thanks 

 

 

this is my page settings 

[Brian Pallas]

I am assuming you want one work offset?  In your Transform Operation Parameters, under Work Offset Numbering, check "Maintain Source Operations". Then under View Manager set a work offset for your initial plane to the appropriate number.  

 

And I believe the Method should be Tool Plane in the Transform Operation Parameters. 

 

(I am still using X7, so I can't be of much help if the software has changed much after this version.  I don't know if it has or not)

[mkd]

did you try selecting "maintain source operatiions" checkbox?

[mirek1017]

thanks guys for the replies.I will try everything tomorrow morning ,but I believe I tried all the options in the rotate windows 

 

thanks one more time 

[MrFish]

really need to see the next page in your rotate parameters too.

[Colin Gilchrist]

Default Horizontal output is generated by using Top WCS, and Front Toolplane. You probably aren't programming with Front plane.

 

Set the Work Offset to Manual, with a value of '0'. Then, use Transform Toolpath to rotate the cuts. There is a Work Offset setting in Transform Toolpath, to 'use source operation's offset'. Something like that. Do not use 'increment' work offset option. 

[mirek1017]

this is my sample file 

 

[Guest]

Try this....

 

Pay attention to the planes change and setting the G54 to 0

 

https://www.dropbox.com/s/wljbyr91tpvoroh/JP_B%20AXIS.mcx-9?dl=0

[Orvie]

For 30 equal instances, your # of transforms should be 29.

Your WCS needs to be Top.

Your work offset should be set to "Manual" & 0.

Posted just fine for me, you will need to add a clearance move between indexes though.

[mirek1017]

 yes ,works now ,this is what I looking for ::))))

 

 

 

thanks guys so much 

 

 

       

[jerms]

Is there a way to do this same thing when using axis substitution? It posts correctly when I turn off substitution, but post the same b value when I use substitution. 

Thanks in advance. 

[Colin Gilchrist]

For Axis Sub, you'll need to physically translate your chains of geometry, and add multiple chains to your Contour path. You cannot "Transform" an Axis Substitution path...

[jerms]

well that's disappointing.. lol. My intent was to rotate (transform) the tool path and post as incremental sub programs. My part has too many details and operations to post out otherwise. Any thoughts?

[Guest]

A real machine will proper memory isn't an option? 

How about a 5 axis multi-surf then transform that?

 

 

[jerms]

29 minutes ago, JParis said:

A real machine will proper memory isn't an option? 

 

 

 

Hard to believe my phone has like 30 million times more memory.

5 axis curve will allow me to do what I'm looking for! Thanks!

[crazy^millman]

3 hours ago, jerms said:

well that's disappointing.. lol. My intent was to rotate (transform) the tool path and post as incremental sub programs. My part has too many details and operations to post out otherwise. Any thoughts?

You can do that just need to approach it different is all. You program your section then use the transform to get the output as the sub programs like you are thinking. Like Colin said unroll the geometry and use it for your axis sub. Then use Axis sub to roll it back. Seems odd, but on your part you just found the better process to get less code using Mastercam.  Moduleworks toolpaths have no filtering what so ever. You get what you get and deal with it. By reverting back to an old school process you are doing it in a way that produces the same quality part, but with far less code. I like Modules works, but been a disconnect in Multi-Axis machining for some years about what is good on the machine for certain application and what is easier to have someone else develop for you. Next hurdle will be when you go to back plot this it should look correct and verify, though I have had issues that have been reported in 2017 and 2018 doing it that were false. When you see a large axis sub look wrong when the back plot is turned on just ignore it. When you run it through the machine sim if you have built your machine then you will get a real idea what is will look like on the machine. You are thinking correctly so proceed on and let us know how it turns out.