UMC 750 ROTARY CUT

[DUM1]

seems like it should be easy ,, I have a part that's outside my travel of course and want to rotary cut the profile and chamfer 

i can get a rotary cut at a b 90 but cant get one at c0 b0

any help would be greatly appreciated 

thanks in advance 

umc tesst ROTARY TEST.mcam

[cncappsjames]

Any chance you've got CAMplete? It's easy to take a contour path and make it spin C-Axis there. 

[GF8er]

20 hours ago, cncappsjames said:

Any chance you've got CAMplete? It's easy to take a contour path and make it spin C-Axis there. 

How is this done in camplete? 

[cncappsjames]

2 hours ago, GF8er said:

How is this done in camplete? 

Do a 2D contour in MC. On the filter page, break arcs into lines. I usually use around .010" because that small is going to look like normal feed lines and typically won't bog down a control as long as it has some sort of look-ahead feature.

Once the project is imported into CAMplete, change the toolpath from a 3+2 to a 5-Axis path then and pick the side where I have enough stroke (say X-) and force it to stay centered on Y and on the X- side. CAMplete then will spin the C-Axis instead of just a profile. 

That's the best way I can explain it not sitting in front of my workstation. 

 

HTH

[Leon82]

I have done that in complete it's in the rotary tab in the cam wizard.

 

[cncappsjames]

25 minutes ago, Leon82 said:

I have done that in complete it's in the rotary tab in the cam wizard.

 

Thanks @Leon82!

[Leon82]

I think there may also be a utility to linearize a tool path but don't remember

[Guest]

2 hours ago, cncappsjames said:

Do a 2D contour in MC. On the filter page, break arcs into lines. I usually use around .010" because that small is going to look like normal feed lines and typically won't bog down a control as long as it has some sort of look-ahead feature.

Once the project is imported into CAMplete, change the toolpath from a 3+2 to a 5-Axis path then and pick the side where I have enough stroke (say X-) and force it to stay centered on Y and on the X- side. CAMplete then will spin the C-Axis instead of just a profile. 

That's the best way I can explain it not sitting in front of my workstation. 

 

HTH

I need to linearize my toolpaths too, I want to do something with the nci positions and its way easier with arcs out of the equation, I imagine it could be programatically set with the sdk.

The camplete sounds pretty great!

[cncappsjames]

1 hour ago, Thee Byte™ said:

The camplete sounds pretty great!

It's BADASS software. Been using it since 2006 and it truly makes 5-Axis programming a pleasurable experience. I can handle tilt/rotation preferences without having to think about Misc.Int/Reals amd making sure I have the right values/bias, etc... 

I just worry about my toolpath... as it should be.

[Colin Gilchrist]

11 hours ago, Thee Byte™ said:

I need to linearize my toolpaths too, I want to do something with the nci positions and its way easier with arcs out of the equation, I imagine it could be programatically set with the sdk.

The camplete sounds pretty great!

Inside the MP Post Language, there is a command variable called 'linarc$', which can be used to break all Arc moves into Line Segments. There are additional 'helper' variables "break lines Type", and "break lines Length" (note: lookup the actual variable names), which give you great control over the arc conversion process.

But that conversion process happens at the Posting level. (NCI Data is still a mix of Arcs and Lines.)

To get your NCI Data into 'only line moves', you have 2 options:

You can disable Arc Output in the Control Definition File, or you can simply program your part with a 5-Axis Toolpath. The 5X paths are all linear (G11) moves in the NCI, with no arc output. You can use the Triangular Mesh path option. This particular 5X path has about 13 different 3X cut-type strategies contained within it. You've got a pocket style, waterline style, horizontal area style, Etc.

Also, in response to your statement about CAMplete, it is literally my favorite Simulation software right now. Having the combination of Machine Kinematic Awareness, Cutting Mode Selection, and the ability to modify the 'output type' on an individual 'path level', makes this one of the best Post Processor solutions on the planet. At Methods, we use CAMplete for most of our machines when possible. 

[Guest]

Just now, Colin Gilchrist said:

You can disable Arc Output in the Control Definition File

Recently, Our post processor was outputting a g2 with no move coordinates on 1 program, not sure why. but the machine complained for obvious reasons, disabling it did the trick.

Just now, Colin Gilchrist said:

Inside the MP Post Language, there is a command variable called 'linarc$', which can be used to break all Arc moves into Line Segments. There are additional 'helper' variables "break lines Type", and "break lines Length" (note: lookup the actual variable names), which give you great control over the arc conversion process.

This is very helpful, I could always read the gcode coordinates back into Mastercam,  that would be slow on larger programs.

 

[sweeper]

Not to hijack the discussion but it seems that camplete is now another software that has been hoovered up by autodesk.  Any changes yet?

[cncappsjames]

None so far that I have noticed. I expect this acquisition to be different than the others.

[gcode]

2 hours ago, cncappsjames said:

None so far that I have noticed. I expect this acquisition to be different than the others.

There will come a time when only AD owned CAM will be supported.

When HSM Works was acquired, Solid Works users were promised support.

Now HSM Works for SW for SW is only available as part of an expensive manufacturing suite

Stand alone HSM Works is no longer available 

 

 

[cncappsjames]

2 hours ago, gcode said:

There will come a time when only AD owned CAM will be supported.

I would rate that statement as extraordinarily unlikely.  Nothing is impossible which is why I won't say that. It would require a rewrite that doesn't make sense to even a company like AD.

It is a non competitive product to any of their offerings or any other product on the market frankly. It's only competition might be ICAM and NC Simul... sort of. Even those aren't really in competition because with those packages you can build your own machines whereas CAMplete cannot. At least for the foreseeable future since the machines are factory verified unlike Vericut, NC Simul, and ICAM.

Post Processing, Collision Checking and Gcode simulation for certain machine tools is what it does. The biggest change I see happening for the foreseeable future is expanding the machine offerings. 

 

I look back at our conversations regarding Dassault's acquisition of SW... a lit of us thought they would kill it off. So far doesn't even look possible at this point and the fact they still haven't killed off using the Parasolid kernel... 

JM2CFWIW 

[DUM1]

thanks for the replies guys 

no I don't have camplete , was lucky to get mastercam , was using ONE CNC for about five years here before I finally talked them in to getting mastercam 

I'm glad it wasn't something stupid simple though since I spent about 4 hours banging my head.

the parts are done but I really need this for me 

On 12/13/2020 at 5:40 AM, Colin Gilchrist said:

or you can simply program your part with a 5-Axis Toolpath. The 5X paths are all linear (G11) moves in the NCI, with no arc output. You can use the Triangular Mesh path option. This particular 5X path has about 13 different 3X cut-type strategies contained within it. You've got a pocket style, waterline style, horizontal area style, Etc.

I've been trying the 5 axis paths and still cant get the effect COLIN, 

I'll keep trying when I have time though ,

This really bugs me because I can program it at the machine but not on mastercam.

[gcode]

a 5X swarf locked to 4 axis with the c/l of the rotary table defined as COR  should give you the code you want 

a lot of this is post dependent... some posts just will not do this. 

[Colin Gilchrist]

30 minutes ago, DUM1 said:

thanks for the replies guys 

no I don't have camplete , was lucky to get mastercam , was using ONE CNC for about five years here before I finally talked them in to getting mastercam 

I'm glad it wasn't something stupid simple though since I spent about 4 hours banging my head.

the parts are done but I really need this for me 

I've been trying the 5 axis paths and still cant get the effect COLIN, 

I'll keep trying when I have time though ,

This really bugs me because I can program it at the machine but not on mastercam.

These 5X paths will produce point-to-point motion. The 'output' formatting, as Tom mentioned, is Post-Dependent. 

The Generic Fanuc 5X Mill Post does not contain any logic to perform this output conversion. My comment was meant more for use with the CAMplete software package, acting as the Post.

[DUM1]

UP DATE !  I think I got it now ,  think this will work ,?

cant wait to try it 

umc tesst ROTARY TEST 2020.mcam

[DUM1]

thanks Colin and G code and everyone else who helped out !

[crazy^millman]

2 hours ago, DUM1 said:

UP DATE !  I think I got it now ,  think this will work ,?

cant wait to try it 

umc tesst ROTARY TEST 2020.mcam

So you are trying to get the table to spin using the Axis of the Table? That is not set to do that. It is set to positioning not substitution. In CAMPLETE you have to enable this function to have it support it. Not to many 5 axis post support this very well either on these types of machines.  I would control this with a 5 Axis toolpath set to 4 Axis verses trying what you are trying. Please let us know if this works, but unless you have a custom post that is being tricked into this from this method from my experience it is not going to work. CAMPLETE allows you to make it happen as I have only even been successful with Mastercam and CAMPLETE doing exactly what you're trying to accomplish without a cheat. How I have done it is make a 4 Axis Definition and use a 4 Axis Post to make code I then copied and pasted into my NC program even then I remember it being a fight to make it happen.

 

[DUM1]

16 hours ago, crazy^millman said:

So you are trying to get the table to spin using the Axis of the Table? That is not set to do that. It is set to positioning not substitution. In CAMPLETE you have to enable this function to have it support it. Not to many 5 axis post support this very well either on these types of machines.  I would control this with a 5 Axis toolpath set to 4 Axis verses trying what you are trying. Please let us know if this works, but unless you have a custom post that is being tricked into this from this method from my experience it is not going to work. CAMPLETE allows you to make it happen as I have only even been successful with Mastercam and CAMPLETE doing exactly what you're trying to accomplish without a cheat. How I have done it is make a 4 Axis Definition and use a 4 Axis Post to make code I then copied and pasted into my NC program even then I remember it being a fight to make it happen.

 

you are correct the original goal of this post was not achievable to mill the profile and chamfer it with the rotary of the table at cobo

 I don't have camplete .

the closest I got was to mill the .015 step with it at 90 and to chamfer it at 90 , which isn't  really what I wanted to do . 

again thanks for trying to helping

[crazy^millman]

59 minutes ago, DUM1 said:

you are correct the original goal of this post was not achievable to mill the profile and chamfer it with the rotary of the table at cobo

 I don't have camplete .

the closest I got was to mill the .015 step with it at 90 and to chamfer it at 90 , which isn't  really what I wanted to do . 

again thanks for trying to helping

Look to using a 4 Axis post for these situations in the future that will output what is needed for a 5 Axis machine. If you don't need the 5 Axis motion per say, but just full 4 Axis then that is a work around. Are you using a 3Rd part post for this machine? If you are everyone I have worked with should be able to help point you in the right direction.

[Colin Gilchrist]

On 12/12/2020 at 8:50 PM, Thee Byte™ said:

I need to linearize my toolpaths too, I want to do something with the nci positions and its way easier with arcs out of the equation, I imagine it could be programatically set with the sdk.

The camplete sounds pretty great!

There is a switch in the MP Post Language to convert lines into arcs. 'linarc$'.