Circular output from Circle 5 Axis Toolpath

[Chipmakr]

I am trying to get circular out put from the multiaxis circlemill toolpath. No matter what machine/post combo I try if I use plain 2d circle mill I get circular output but as soon as I try to use the multiaxis circlemill toolpath all I get is lines. Is there somewhere i can change this. I am most concerned with getting my mpgen5x_millplus machine def to accomplish this.

 

TIA

[mayday]

Use the g68 rotaion in the misc values.

this is from our E420H Mazak pst. on the sub spindle

Ignor the macro, I hand coded that in

 

 

 

N671(5/8 CARBIDE ENDMILL W/.01 RAD. - FINISH SCALLOPS)

G20 G10.9 X0

G91 G28 X0.

G28 Y0. Z0.

M902

G0 G90 G55 U0.

T74.01 T1 M06

M300

G97 S1220 M03

M108 M312

G0 G90 G53 B90.

M107 M310

G55

G68 X0. Y0. Z0. I0. J1. K0. R90.

G17

U0.

X-.383 Y-3.5106

G90 G43 Z4.

#100=1

WHILE[#100LE16]DO1

(FINISH 32 SCALLOPS)

X-.383 Y-3.5106 M08

Z0.

G94 G1 G41 X-.2561 Y-3.4825 F6.

G3 X-.2999 Y-3.4198 R.1

X-.39 Y-3.3935 R.1675

X-.4801 Y-3.4198 R.1675

X-.524 Y-3.4825 R.1

G1 G40 X-.397 Y-3.5106

X-.383

G41 X-.2561 Y-3.4825

G3 X-.2999 Y-3.4198 R.1

X-.39 Y-3.3935 R.1675

X-.4801 Y-3.4198 R.1675

X-.524 Y-3.4825 R.1

G1 G40 X-.397 Y-3.5106

G0 Z4.

M312

G0 G91 U7.5

M310

G90

G0 Z4.

X-.975 Y-3.5103

Z0.

G1 G41 X-.8493 Y-3.4772

G3 X-.8957 Y-3.4163 R.1

X-.98 Y-3.3935 R.1675

X-1.0643 Y-3.4163 R.1675

X-1.1107 Y-3.4772 R.1

G1 G40 X-.985 Y-3.5103

X-.975

G41 X-.8493 Y-3.4772

G3 X-.8957 Y-3.4163 R.1

X-.98 Y-3.3935 R.1675

X-1.0643 Y-3.4163 R.1675

X-1.1107 Y-3.4772 R.1

G1 G40 X-.985 Y-3.5103

G0 Z4.

M312

G0 G91 U15.

M310

G90

#100=#100+1

END1

G0 G90 Z5.M9

G69

M312

G91 G28 X0.

G28 Y0. Z0. M305

G90 G53 B0.

M99

%

[Chipmakr]

I should expalin my situation a little better. I am using this mpgen5x_millplus machine def to post out an NCI file. Then actually using this NCI file to generate my posted .H code in CamPlete. My toolpath backplots lines and the resolution is not as fine as I would like.I am using this machine def anytime I have 5 axis moves or in this case I want the Multiaxis circlemill to feed to vector information through the NCI so I don't have to create all the WCS planes needed for each hole orientation. I used the verisurf hole axis to create all my hole information and then simply used this one toolpath to get all the hole & vector information I needed. In the past I have been creating WCS's for each unique oreintation and the using 2d contour to get the motion I wanted. I really like that with the verisurf/ circle 5 axis method it only takes a few simple steps to get my holes programmed I just wish I could get circular output instead of these faceted lines. I don't see anyplace to input a tolerance inside the Circle 5 axis toolpath atleast if I could do that I could get the resolution of these small lines moves down to a reasonable level.

[mayday]

thinking........

have you tried FBM for the holes? It wil create the WCS planes for you although I haven't used it for 5x stuff, only 4x

I dont think you will get circle output without using G68 rotation. otherwise its crossing the axis planes and has to break it up into lines

[Chipmakr]

I dont have a "G68" option on my misc values page. Would setting a value in the misc values page effect the output of the NCI or would it just determine how the NCi was handled once it actually runs thru the post processor?

[Guest CNC Apps Guy 1]

Let's back up for a second...

 

In CAMplete, there are some settings in the Advanced Settings page. When I get into the office later this morning, I'll post them here for you.

[gcode]

I havn't looked, but I'm guessing that the Mastercam NCI is point to point.

and that's what's going to get posted reguardless of post settingsd

[Guest CNC Apps Guy 1]

Here's the skinny,

 

1. Open up CAMplete. Don't open any files or anything.
2. Go to Tools, Options.
3. Click Back Up Installation. This will allow you to go back to your previous settings.
4. Click on the "Advanced tab. You'll get a warning message basically telling you to not change ANY values unless you know what you're doing or have been advised by a CAMplete support analyst. Click OK.
5. Find the "CAM Operations" section and expand it,there are a few things you'll need to check/uncheck/modify. Expand this section to see the options.
6. Check "EXPEREMENTAL 360 Deg. Arc Processing"
7. Check "EXPEREMENTAL Helical Milling Processing"
8. Collapse the "CAM Operations" section
9. Find the "CAMFileIOPrefs" section and expand it, there are a few things you'll need to check/uncheck/modify. Expand this section to see the options.
10. Convert Helixes To Points when loading - Uncheck this.
11. Helical Milling - Filter... - Check this.

That shoud ldo it on the CAMplete side.

 

On the Mastercam side, in your Control Def, under the "Arc" Control Topic, you need to have Allow 360 Deg. Arcs set in all axes, don;t break for X and Y and break at 180 for the XZ and YZ planes. Support arcs in all planes. Suppport Helix in all planes.

 

Thant shoudl do it.

 

HTH

 

 

[Chipmakr]

James, Gcode, & Wes thanks for taking time to help me out.

 

I do not have the "Helical Milling - Filter" in my "CAMFileIOPrefs". I am running CP version "4.1.255 PR3 unicode". So thats probably an update that was added since my maintainence ran out. All my settings in MC were as you suggested except for "break at 180 for the XZ and YZ planes" which I changed. I am still getting linear output for a 2d circle. Since there is no helical motion for CP to deal with the import log shows no signs of conversion for helical moves, so I don't think the "Helical Milling - Filter" will help me anyway until I can get something other than linear 2d moves out of MC.

 

Is this toolpath just made this way? Its seems that since you simply input a circle diameter that it would be easy to get circular output.

[CJep]

Dwain,

Currently the 5axis circmill toolpaths output in linear code, to get the helical output you will need create a custom toolplane normal to the hole vector and use a standard circmill toolpath.

[Guest CNC Apps Guy 1]

I am running CP version "4.1.255 PR3 unicode".

 

I looked that up and WOW... just WOW!!! That came out between February and March of 2008. You may want to hit up the boss for maintenance. I don't know what it will run, but they have added a TON of new features.

 

FWIW...I'm running V4.5.396

[Chipmakr]

The last time I spoke to Paul they were added macro support and alot of other cool stuff. Unfortunatley it was on the chopping block whne times got hard. With MC and Calypso maint. coming first it will probably be a tough sell to get back onto it. We have to go thru George Fischer when we do it as well and they are very proud of anything they sell you

 

It's dissappointing that the circle toolpath will not output circle moves. It is such a quick way to program.