Where to start? rotary program

[CNCZACK]

im programming this on a 4th axis rotary machine. I havent messed with this machine in the last year and all previous program has been simple mill off lugs. this one is a little more complex but im not sure where to start? do i unroll my geometry? do i use optirough? anyone have any good starting point suggestions? i dont have any multi axis toolpaths available. only standard basic mastercam.

 

 

 

4TH AXIS.mcam

[crazy^millman]

3+1 and Axis Substitution will be your friend here. Take the two section in between the two bosses and xform unroll the shape and then can use what ever 3 Axis toolpath you would want in a 4 Axis output to rough and finish them in. They will not be normal to the walls they will be normal to the floor. Then you use a Stock model to see the left over stock and finish the vertical walls at A0 and A180. Using a 3/8 ball endmill will eliminate any transition between both areas and the rest is just rotated planes.

[CNCZACK]

32 minutes ago, crazy^millman said:

3+1 and Axis Substitution will be your fried here. Take the two section in between the two bosses and xform unroll the shape and then can use what ever 3 Axis toolpath you would want in a 4 Axis output to rough and finish them in. They will not be normal to the walls they will be normal to the floor. Then you use a Stock model to see the left over stock and finish the vertical walls at A0 and A180. Using a 3/8 ball endmill will eliminate any transition between both areas and the rest is just rotated planes.

So when you mention finishing at A0 and A180 what do you mean by this? also should i be looking at creating wire frame from the inside of the radii like this... ? 

[crazy^millman]

4 hours ago, CNCZACK said:

So when you mention finishing at A0 and A180 what do you mean by this? also should i be looking at creating wire frame from the inside of the radii like this... ? 

No just of the floor section for the Axis sub. Looking at the view you have 2 walls on each side of this rib at this position which on the Machine would be A0 then the other side of the part would be A180. Then the hole across that rib would be at A90.

[CNCZACK]

On 2/21/2022 at 7:13 PM, crazy^millman said:

No just of the floor section for the Axis sub. Looking at the view you have 2 walls on each side of this rib at this position which on the Machine would be A0 then the other side of the part would be A180. Then the hole across that rib would be at A90.

I cant get the program on here because of the size but ive added a picture to help explain. Ive got this thing pretty much roughed out except  the walls of the boss. you can see in the picture ive attached there is a good bit of material on both sides of the boss. on the left side i unrolled my geometry and used a ball mill to get it closer but i still cant seem to figure out what to use to get the walls closer to finished or even finished at all here. do you have any suggestions? https://ibb.co/vPZ6tQf

[crazy^millman]

21 minutes ago, CNCZACK said:

I cant get the program on here because of the size but ive added a picture to help explain. Ive got this thing pretty much roughed out except  the walls of the boss. you can see in the picture ive attached there is a good bit of material on both sides of the boss. on the left side i unrolled my geometry and used a ball mill to get it closer but i still cant seem to figure out what to use to get the walls closer to finished or even finished at all here. do you have any suggestions? https://ibb.co/vPZ6tQf

Like i said you will leave two wedge shapes at those walls using the 4th Axis process. Now in 3+1 at the A0 View you can do a simple 3D OPTI-REST using a stock model to rough the excess material at the A0 and A180 positions. Then come back and finish those sections. I can write a 4th Axis toolpath to cut all of that in one finish operation, but sorry I just don't have much time this week to help. With MultiAxis Toolpaths all of this would take minutes to program.

[crazy^millman]

Zack, see if this help you out. Please review and let me know if you have any questions. I have only use 3 Axis toolpaths to rough and finish what i did the in the file. Many people don't think about the fact you can surface machine flat surfaces with a contour toolpath. I used it to make a flowline or parallel style toolpath, but have it start in the center and work out. We lost Negative Lead In-Out to get the tool in and out of the cut really nicely. I couldn't cheat the toolpath editor to get what I wanted to get in and out like we could do in previous version. I have tested in Beta 2023 and Negative Lead in and out is fixed. 

The other thing is the code will be very clean and nice for the 4th axis and should run really good.

5th Axis Help for a 4th Axis Part

[CNCZACK]

On 2/25/2022 at 3:30 PM, crazy^millman said:

Zack, see if this help you out. Please review and let me know if you have any questions. I have only use 3 Axis toolpaths to rough and finish what i did the in the file. Many people don't think about the fact you can surface machine flat surfaces with a contour toolpath. I used it to make a flowline or parallel style toolpath, but have it start in the center and work out. We lost Negative Lead In-Out to get the tool in and out of the cut really nicely. I couldn't cheat the toolpath editor to get what I wanted to get in and out like we could do in previous version. I have tested in Beta 2023 and Negative Lead in and out is fixed. 

The other thing is the code will be very clean and nice for the 4th axis and should run really good.

5th Axis Help for a 4th Axis Part

Wow, this is way above and beyond. I appreciate this so much! im going to make sure i save this into my notes and to study these toolpaths for the future.

I do have one problem and im having mcam post check into it. when its out on the machine it doesnt rotate to the shortest distance so it will go almost a full 360 before getting back to position as well as the output feed rate for the rotary. i did change some machine definitions to try and correct it but i think they will have some adjustments on their end to correct it. none the less these are minor in the grand scheme of things as we ramp up to running this machine full time again. 

[crazy^millman]

4 hours ago, CNCZACK said:

Wow, this is way above and beyond. I appreciate this so much! im going to make sure i save this into my notes and to study these toolpaths for the future.

I do have one problem and im having mcam post check into it. when its out on the machine it doesnt rotate to the shortest distance so it will go almost a full 360 before getting back to position as well as the output feed rate for the rotary. i did change some machine definitions to try and correct it but i think they will have some adjustments on their end to correct it. none the less these are minor in the grand scheme of things as we ramp up to running this machine full time again. 

Hand edit what you need on the machine to make it the most efficient process possible. Mastercam doesn't take kinematics into account and this method I used is so far off the beaten path no where for it to really do so.

I share my knowledge to help in real world conditions not made up demos or canned presentations to wazzel and dazzel people. Here was a prime example of the power of Mastercam. What is odd compare what I did with the newest most advanced Multiaxis toolpaths Mastercam has these old methods kick them to the curb. They produce cleaner more efficient motion and code. Crazy filtering was added to improve Mastercam and around X5 they tore it up badly. We got locked WCS planes about then to fix the floating issues we had that was crashing Mastercam and required you to move everything to TOP/TOP/TOP for 5 Axis toolpaths. I have shared plenty of examples and I think finally people are listening to my crazy talk and seeing Math don't lie.

Please take what I share and pass it on to others. Help them grow and be better. I always learn more helping and teaching others doing something. This reminded me of what we use to do and how much stock models and other things have helped the programming process over the years. In the past I would have solid modeled all of this to have a model to help me know what the stock model gave me in a few seconds. Yes I am that crazy programmer who looks for every possible thing to cut every possible second out of a program when given the right amount of time to do so.

[Jespertech]

I'm currently loving this post because I've been needing more experience in axis substitution for more advanced rotary work. 

Once again Ron went above and beyond in providing some deep cut  experience in doing this type of work.  I do have some questions regarding the unrolled surfaces you created for toolpathing this. I gave it my best to recreate the process and I think I'm close but I also feel like I'm taking the extreme long road to get there.

There are also differences in my surface compared to yours where as yours is much more comparable to the actual features of the part. If you could spare just a few more moments of your time to explain how you went about creating the surfaces it would be greatly appreciated. 

I'll include an image of what I did for comparison.

Thanks in advance.

[Jespertech]

here's a better view of the surface I created.

[crazy^millman]

23 minutes ago, Jespertech said:

here's a better view of the surface I created.

I was typing this answer then stepped away and came back and you added the above screen shot.

I took the floor shape and unrolled it. I then offset the shape the .1875 that is the fillet and then filleted the sharp corners the .1875. Once the outside shape was created I then used surface Extrude to make the Surfaces. This is similar to solid extrude where you get a close shape, I could have made this with solids then made surfaces from the solid shape, but since I have worked with surface models for over 30 years not a big deal to just work with surfaces. I then removed the top surface and filleted the floor sharp corners to represent the shape of the part that is rolled now unrolled. 

I also did toolpaths where I drove the round part using the Unroll on the round model.

Another way to drive this toolpath is with surfacing toolpaths like I did with contour. In the old school toolpaths you have to click on the rotary axis, but it has been tore up for many versions and I quit using it years ago why I went with the contour toolpath like I did to mimic them.

[Jespertech]

13 minutes ago, crazy^millman said:

I was typing this answer then stepped away and came back and you added the above screen shot.

I took the floor shape and unrolled it. I then offset the shape the .1875 that is the fillet and then filleted the sharp corners the .1875. Once the outside shape was created I then used surface Extrude to make the Surfaces. This is similar to solid extrude where you get a close shape, I could have made this with solids then made surfaces from the solid shape, but since I have worked with surface models for over 30 years not a big deal to just work with surfaces. I then removed the top surface and filleted the floor sharp corners to represent the shape of the part that is rolled now unrolled. 

I also did toolpaths where I drove the round part using the Unroll on the round model.

Another way to drive this toolpath is with surfacing toolpaths like I did with contour. In the old school toolpaths you have to click on the rotary axis, but it has been tore up for many versions and I quit using it years ago why I went with the contour toolpath like I did to mimic them.

Perfect!  the missing link for me was the "surface extrude" which was exactly what I was trying to recreate through flat boundary and loft. Which eventually did work but that coupled with me having to add wireframe and sweep for the rads' was about 5 steps longer then what you just taught me. Thank you very much for the help. It'll certainly save countless hours and headaches for me in the future.

[crazy^millman]

51 minutes ago, Jespertech said:

Perfect!  the missing link for me was the "surface extrude" which was exactly what I was trying to recreate through flat boundary and loft. Which eventually did work but that coupled with me having to add wireframe and sweep for the rads' was about 5 steps longer then what you just taught me. Thank you very much for the help. It'll certainly save countless hours and headaches for me in the future.

Sorry, but this is the kind of teaching that is missing on so many of the sites. Modeling basics that are still needed. Model Prep and other tools are awesome additions to the software, but not every company can afford the full package of Mastercam. Like I said these older methods still shine in certain situations over the most advanced toolpaths any CAM system has to offer from a code stand point. I want to rotate the A Axis one time move over in Y and then rotate it back and that should be 3 lines of code without having to jump through any hoops. Should should be pretty straight forward with any of the most advanced 5 Axis toolpaths. Nope I have to go through 20 dialogs to do exactly what we did with basic 2d Contour here. Having come from Pencil and Paper background 30+ years for making CNC Programs I always looked for cheats and process to reduce the process and the amount of work it took to make a program. If I could write a macro to surface machine a shape like this I did that. I added that process using Transform Rectangular and Transform Rotate the shared file. Re download it and see what I have added. Generic Post says it is not supported. Here is just the 1st Section from a Generic HAAS 4 Axis post.

 

%
O2020
(4TH AXIS 1ST SUB LOOP)
(DATE=DD-MM-YY - 03-03-22 TIME=HH:MM - 08:34)
(MCX FILE - F:\DROPBOX\EMASTERCAM\4TH AXIS 5TH AXIS HELP.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\4TH AXIS )
(MATERIAL - ALUMINUM INCH - 2024)
(T2|3/8 BALL ENDMILL|H2|D2|TOOL DIA. - .375)
N100 G20
N110 G94 G1 G17 G40 G49 G80 G90 F72.
N120 T2 M6
N130 G187 P3 E.001
N140 G94 G1 G90 G54 X-2.0061 Y0. A25.678 S6000 M3 F72.
N150 G43 H2 Z2.2441
N160 M98 P2021
N230 G90 X-1.9861 F72.
N240 M98 P2021
N310 G90 X-1.9661 F72.
N320 M98 P2021
N390 G90 X-1.9461 F72.
N400 M98 P2021
N470 G90 X-1.9261 F72.
N480 M98 P2021
N550 G90 X-1.9061 F72.
N560 M98 P2021
N630 G90 X-1.8861 F72.
N640 M98 P2021
N710 G90 X-1.8661 F72.
N720 M98 P2021
N790 G90 X-1.8461 F72.
N800 M98 P2021
N870 G90 X-1.8261 F72.
N880 M98 P2021
N950 G90 X-1.8061 F72.
N960 M98 P2021
N1030 G90 X-1.7861 F72.
N1040 M98 P2021
N1110 G90 X-1.7661 F72.
N1120 M98 P2021
N1190 G90 X-1.7461 F72.
N1200 M98 P2021
N1270 G90 X-1.7261 F72.
N1280 M98 P2021
N1350 G90 X-1.7061 F72.
N1360 M98 P2021
N1430 G90 X-1.6861 F72.
N1440 M98 P2021
N1510 G90 X-1.6661 F72.
N1520 M98 P2021
N1590 G90 X-1.6461 F72.
N1600 M98 P2021
N1670 G90 X-1.6261 F72.
N1680 M98 P2021
N1750 G90 X-1.6061 F72.
N1760 M98 P2021
N1830 G90 X-1.5861 F72.
N1840 M98 P2021
N1910 G90 X-1.5661 F72.
N1920 M98 P2021
N1990 G90 X-1.5461 F72.
N2000 M98 P2021
N2070 M5
N2080 G91 G0 G28 Z0.
N2090 G28 X0. Y0. A0.
N2100 M30
 
O2021
N170 G91
N180 A128.644 F1838.3
N190 X-.01 F72.
N200 A-128.644 F1838.3
N210 G90
N220 M99
%

25 Years ago on a HAAS we handled it this way.

%
O2020
(4TH AXIS 1ST SUB LOOP)
(DATE=DD-MM-YY - 03-03-22 TIME=HH:MM - 08:34)
(MCX FILE - F:\DROPBOX\EMASTERCAM\4TH AXIS 5TH AXIS HELP.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\4TH AXIS )
(MATERIAL - ALUMINUM INCH - 2024)
(T2|3/8 BALL ENDMILL|H2|D2|TOOL DIA. - .375)
N100 G20
N110 G94 G1 G17 G40 G49 G80 G90 F72.
N120 T2 M6
N130 G187 P3 E.001
N140 G94 G1 G90 G54 X-2.0061 Y0. A25.678 S6000 M3 F72.
N150 G43 H2 Z2.2441
N160 M98 P2021 L24
N2070 M5
N2080 G91 G0 G28 Z0.
N2090 G28 X0. Y0. A0.
N2100 M30
 
O2021
N170 G91
N180 A128.644 F1838.3
N190 X-.01 F72.
N200 A-128.644 F1838.3
N201 X-.01 F72.(RDB SHIFTED ADDED FOR LOOP)
N210 G90
N220 M99
%

I added the last X-.01 needed to move the sub over the needed shift for the 24 times to repeat the sub program. I could have handled that with the chain I made, but then the way Mastercam handles this would be wrong Here is a small program we have achieved a really clean code process that will kick any Advance Multi Axis toolpath to the curb in speed and running on any machine. I dare anyone to prove to me that 10,00,000 lines of code will make a better part cutting this same area. Again where Math don't line!!!!

[Jespertech]

34 minutes ago, crazy^millman said:

Sorry, but this is the kind of teaching that is missing on so many of the sites. Modeling basics that are still needed. Model Prep and other tools are awesome additions to the software, but not every company can afford the full package of Mastercam. Like I said these older methods still shine in certain situations over the most advanced toolpaths any CAM system has to offer from a code stand point. I want to rotate the A Axis one time move over in Y and then rotate it back and that should be 3 lines of code without having to jump through any hoops. Should should be pretty straight forward with any of the most advanced 5 Axis toolpaths. Nope I have to go through 20 dialogs to do exactly what we did with basic 2d Contour here. Having come from Pencil and Paper background 30+ years for making CNC Programs I always looked for cheats and process to reduce the process and the amount of work it took to make a program. If I could write a macro to surface machine a shape like this I did that. I added that process using Transform Rectangular and Transform Rotate the shared file. Re download it and see what I have added. Generic Post says it is not supported. Here is just the 1st Section from a Generic HAAS 4 Axis post.

 

%
O2020
(4TH AXIS 1ST SUB LOOP)
(DATE=DD-MM-YY - 03-03-22 TIME=HH:MM - 08:34)
(MCX FILE - F:\DROPBOX\EMASTERCAM\4TH AXIS 5TH AXIS HELP.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\4TH AXIS )
(MATERIAL - ALUMINUM INCH - 2024)
(T2|3/8 BALL ENDMILL|H2|D2|TOOL DIA. - .375)
N100 G20
N110 G94 G1 G17 G40 G49 G80 G90 F72.
N120 T2 M6
N130 G187 P3 E.001
N140 G94 G1 G90 G54 X-2.0061 Y0. A25.678 S6000 M3 F72.
N150 G43 H2 Z2.2441
N160 M98 P2021
N230 G90 X-1.9861 F72.
N240 M98 P2021
N310 G90 X-1.9661 F72.
N320 M98 P2021
N390 G90 X-1.9461 F72.
N400 M98 P2021
N470 G90 X-1.9261 F72.
N480 M98 P2021
N550 G90 X-1.9061 F72.
N560 M98 P2021
N630 G90 X-1.8861 F72.
N640 M98 P2021
N710 G90 X-1.8661 F72.
N720 M98 P2021
N790 G90 X-1.8461 F72.
N800 M98 P2021
N870 G90 X-1.8261 F72.
N880 M98 P2021
N950 G90 X-1.8061 F72.
N960 M98 P2021
N1030 G90 X-1.7861 F72.
N1040 M98 P2021
N1110 G90 X-1.7661 F72.
N1120 M98 P2021
N1190 G90 X-1.7461 F72.
N1200 M98 P2021
N1270 G90 X-1.7261 F72.
N1280 M98 P2021
N1350 G90 X-1.7061 F72.
N1360 M98 P2021
N1430 G90 X-1.6861 F72.
N1440 M98 P2021
N1510 G90 X-1.6661 F72.
N1520 M98 P2021
N1590 G90 X-1.6461 F72.
N1600 M98 P2021
N1670 G90 X-1.6261 F72.
N1680 M98 P2021
N1750 G90 X-1.6061 F72.
N1760 M98 P2021
N1830 G90 X-1.5861 F72.
N1840 M98 P2021
N1910 G90 X-1.5661 F72.
N1920 M98 P2021
N1990 G90 X-1.5461 F72.
N2000 M98 P2021
N2070 M5
N2080 G91 G0 G28 Z0.
N2090 G28 X0. Y0. A0.
N2100 M30
 
O2021
N170 G91
N180 A128.644 F1838.3
N190 X-.01 F72.
N200 A-128.644 F1838.3
N210 G90
N220 M99
%

25 Years ago on a HAAS we handled it this way.

%
O2020
(4TH AXIS 1ST SUB LOOP)
(DATE=DD-MM-YY - 03-03-22 TIME=HH:MM - 08:34)
(MCX FILE - F:\DROPBOX\EMASTERCAM\4TH AXIS 5TH AXIS HELP.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\4TH AXIS )
(MATERIAL - ALUMINUM INCH - 2024)
(T2|3/8 BALL ENDMILL|H2|D2|TOOL DIA. - .375)
N100 G20
N110 G94 G1 G17 G40 G49 G80 G90 F72.
N120 T2 M6
N130 G187 P3 E.001
N140 G94 G1 G90 G54 X-2.0061 Y0. A25.678 S6000 M3 F72.
N150 G43 H2 Z2.2441
N160 M98 P2021 L24
N2070 M5
N2080 G91 G0 G28 Z0.
N2090 G28 X0. Y0. A0.
N2100 M30
 
O2021
N170 G91
N180 A128.644 F1838.3
N190 X-.01 F72.
N200 A-128.644 F1838.3
N201 X-.01 F72.(RDB SHIFTED ADDED FOR LOOP)
N210 G90
N220 M99
%

I added the last X-.01 needed to move the sub over the needed shift for the 24 times to repeat the sub program. I could have handled that with the chain I made, but then the way Mastercam handles this would be wrong Here is a small program we have achieved a really clean code process that will kick any Advance Multi Axis toolpath to the curb in speed and running on any machine. I dare anyone to prove to me that 10,00,000 lines of code will make a better part cutting this same area. Again where Math don't line!!!!

I couldn't agree more, and is one of the reasons I believe strongly in teaching my apprentices how to code by hand long before they jump into Mastercam. Having that understanding from the inside out is so crucial for success especially when you're responsible for another person running your code. 

In regards to modeling I've always taken it upon myself to model the majority of the parts I make. At first I caught some flack from my fellow programmers who didn't understand why I wasn't solely dependent on the customer provided models. But once I started getting really good and showing the powers of manipulation to get the most out of my toolpaths they were coming to me to make their lives easier. I also hate how most models don't hold true to pre-plate tolerances and other print designated specifications. So topics like these are often my favorite because it helps blend the two worlds for me and allows me to really learn not only better modeling practices but better programming as well. 

so once again, I tip my hat to you sir and all the other people on this forum who take the time to help.

[crazy^millman]

Bump someone recently liked this topic and it has some good information in it. The link I shared is still good.