[Xavior]

Hi Guys,

Well im back with a new adventure and this time its to streamline my programming and condense the length of my programs. Currently, when programming, lets say an interpolation of a hole, it would spit out thousands of lines of xyz of points which makes edition the program impossible on the control.

Here is the idea, does anyone know how i can go about enabling canned cycles or is that something that i must program in? Would love to see the programs much shorter as space is always an issue with a control. Is this something that must also be edited into the post for my haas machine?

Thanks in advance

[neurosis]

Sounds like you need to edit your control definition. Open your control definition for which ever machine you are using and make sure that in the "ARC" settings that you have "support arcs in XY plane" checked. If your machine is able to helix you can check which planes your machine is capable of that in as well.


If you are using a Circle Mill tool path make sure that you have "output arc moves" checked.

[Xavior]

Sounds like you need to edit your control definition. Open your control definition for which ever machine you are using and make sure that in the "ARC" settings that you have "support arcs in XY plane" checked. If your machine is able to helix you can check which planes your machine is capable of that in as well.


If you are using a Circle Mill tool path make sure that you have "output arc moves" checked.

Hi,

Just checked to see whats was checked off and i have:

Supports XY
Supports XZ
Support YZ

But when i post my program, im stil getting thousands of lines of xyz coordinates. Any ideas how i should be setting my tools up or if im missing something specific?

[cadcam]

are you using helix entry as contouring a hole would not give you this unless you are using say Helix Bore

[Superman]

The Filter and Tolerance areas control toolpath ajustment to give arcs

For all operations , those areas suggested must be enabled in the control definition, plus the filter / tolerance should also be checked ON ( as well as the planes -XY at the very minimum ) to allow Mastercam to be able to adjust that particular toolpath to give arcs

NOTE--any splines that are used in a contour WILL give point to point code...these need to be "Simplified" ( under "Edit" pull-down ), splines may need to be broken into shorter segments before the simplify operation
eg. a horseshoe shape would need major ajustment to form an arc, but breaking it up would turn allow it to turn into a series of arcs that is much closer to the original shape.

[Xavior]

The Filter and Tolerance areas control toolpath ajustment to give arcs

For all operations , those areas suggested must be enabled in the control definition, plus the filter / tolerance should also be checked ON ( as well as the planes -XY at the very minimum ) to allow Mastercam to be able to adjust that particular toolpath to give arcs

NOTE--any splines that are used in a contour WILL give point to point code...these need to be "Simplified" ( under "Edit" pull-down ), splines may need to be broken into shorter segments before the simplify operation
eg. a horseshoe shape would need major ajustment to form an arc, but breaking it up would turn allow it to turn into a series of arcs that is much closer to the original shape.

The filter and tolerances have some interesting options:

Filter Ratio is currently set to off, but we have 1:1, 2:1, 3:1 and custom

Once you pick one of those options you have the ability to check off where you want to create the arcs. I did try to pick 1:1 and reposted the program and it reduced the program from 1700 lines to 1200 lines but although the program was still giving me the xyz points output for that tool that was arcing. Any Ideas?

Not sure what im doing wrong but i went in to the control definition and turned on helix support as well in as planes. Not sure if i have helix support but its a haas vf5.

Would love to ideally see a canned program where it does not run 1000 lines of xyz of code.


Here is a sample of my program it posted:

()
( FACE MILL 1.25 TOOL - 21 DIA. OFF. - 21 LEN. - 21 TOOL DIA. - 1.25 )
N740 T21 M6
()
N750 G0 G90 G54 X1.455 Y-1. C0. S1069 M3
N760 G43 H21 Z.25
N770 M88
N780 Z.2
N790 G1 Z0. F10.
N800 G41 D21 X1.4568 Y-1.0127 Z-.0023 F12.8
N810 X1.4621 Y-1.0243 Z-.0045
N820 X1.4705 Y-1.034 Z-.0068
N830 X1.4813 Y-1.0409 Z-.0091
N840 X1.4936 Y-1.0445 Z-.0114
N850 X1.5064 Z-.0136
N860 X1.5187 Y-1.0409 Z-.0159
N870 X1.5295 Y-1.034 Z-.0182

^^ thats the tool that is arcing

The last tool in my program is now getting I's and J's added to it as it was not there before. See Below:

( TOOL - 23 DIA. OFF. - 23 LEN. - 23 TOOL DIA. - 1. )
N1740 T23 M6
()
N1750 G0 G90 G54 X1.5 Y-1. C0. S1000 M3
N1760 G43 H23 Z.25
N1770 M8
N1780 Z.1
N1790 G1 Z.0417 F10.
N1800 G42 D23 Y-.86 F5.
N1810 G2 X1.5274 Y-.8573 Z.0371 I.0274 J-.14
N1820 X1.67 Y-1. Z0. I0. J-.1427
N1830 X1.5 Y-1.17 Z-.0417 I-.17 J0.


Any ideas on how i can improve the situation?

[Xavior]

are you using helix entry as contouring a hole would not give you this unless you are using say Helix Bore

Not sure what you mean by that as if a helix entry is when you plunge down at the same time than no, im more so using arc entry in.

[Xavior]

Sounds like you need to edit your control definition. Open your control definition for which ever machine you are using and make sure that in the "ARC" settings that you have "support arcs in XY plane" checked. If your machine is able to helix you can check which planes your machine is capable of that in as well.


If you are using a Circle Mill tool path make sure that you have "output arc moves" checked.

I have the supports arcs checked in all 3 areas, xy, xz yz but i dont see where this "output arcs" is

[Xavior]

Ill post up my mastercam drawing file for you guys to download and see where im going wrong here... please see link:


http://dl.dropbox.com/u/24570519/TFX-PT-0000021-B.MCX-5

[Superman]

Filter Ratio is currently set to off, but we have 1:1, 2:1, 3:1 and custom

Would love to ideally see a canned program where it does not run 1000 lines of xyz of code.

OK, I think I may know the problem.......terminology
canned cycles = usually holemaking, drilling, tapping, reaming boring etc
G2/G3 are not canned cycles, but being able to define a "macro" to machine a shape is possible ( within reason, & verry difficult- a custom post would be needed = $$$ )

mastercam toolpaths are all point to point paths
until the following are ON

"Filter" - used in wireframe operation generally
- filter ON, & "Allow arcs XY/XZ/YZ" ( any or all of these ON ) plus the "support arcs" has to be permitted in the control definition
"Tolerance" - used in surfacing, or multi-axis paths
( OFF = point to point paths, 1:1 etc = allows the points to be more spaced out & then allows those new paths to be "ajusted" again for the fitting of arcs

The numbers used in these areas relate to "how much" mastercam can "adjust" the calculated paths to be able to fit an arc
- smaller number = the more accurate the path, & larger NC file
- larger number = more "cuspy" ( flats ), least accurate, & smaller NC file

If you need short NC files, then you have to use operations that can output them ie 2D_Contour, 2D_Pocket, facing etc