Arcs not being outputted for surfacing

[Guess_who]

Has anyone else noticed that in X7 when you do surfacing that should create arcs, it actually creates point to point instead.

 

Just pick a cone like a large chamfer and try to surface it. In X6 flowline would output arcs, but now, no matter what I do, X7 outputs a bucket load of lines.

And I can't get it to create arcs.

 

 

 

And just to vent for a minute, maybe I'm dense but what's the point of MasterCam treating my check surfaces as drive surfaces in all of the surface high speed cycles . I just want to tell the endmill not to hit some surrounding surfaces. but it insists on surfacing all my check surfaces. I have to use the old cycles to avoid this. How does that make any sense. Maybe I'm missing the point.

 

 

 

MasterCam X7, MU1

[crazy^millman]

Has anyone else noticed that in X7 when you do surfacing that should create arcs, it actually creates point to point instead.

 

Just pick a cone like a large chamfer and try to surface it. In X6 flowline would output arcs, but now, no matter what I do, X7 outputs a bucket load of lines.

And I can't get it to create arcs.

 

What do you have your arc settings set to for the operation you are using? Here is your example with arcs no problem X7MU1 and what I did was 4 different settings on the filters for you to see what happens.

 

Here is what 25-75 gives for output.

 

O0000(ARC_OUTPUT 25-75)
(DATE=DD-MM-YY - 26-02-14 TIME=HH:MM - 15:18)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MCAMX7\MCX\5TH AXIS FLOWLINE ARC OUTPUT.MCX-7)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAMX7\MILL\NC\ARC_OUTPUT 25-75.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T256 | 1/2 BALL ENDMILL | H256 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
( 25-75 FILTER APPLIED )
N120 T256 M6
N130 G0 G90 G54 X.7003 Y-.02 A0. S1069 M3
N140 G43 H256 Z2.15
N150 Z2.
N160 G1 Z1.9 F6.42
N170 X.7 Y0.
N180 G3 X-.7 I-.7 J0.
N190 X.7 I.7 J0.
N200 G1 X.7003 Y.02
N210 X.7303 Z1.86
N220 X.73 Y0.
N230 G2 X-.73 I-.73 J0.
N240 X.73 I.73 J0.
N250 G1 X.7303 Y-.02
N260 X.7603 Z1.82
N270 G3 X-.7597 Y.0216 I-.76 J.0196
N280 X.7597 Y-.0216 I.7597 J-.0216
N290 G1 X.76 Y0.
N300 X.7603 Y.02
N310 X.7903 Z1.78
N320 X.79 Y0.
N330 G2 X-.79 I-.79 J0.
N340 X.79 I.79 J0.
N350 G1 X.7903 Y-.02
N360 X.8203 Z1.74
N370 G3 X-.8197 Y.0233 I-.82 J.0197
N380 X.8187 Y-.0469 I.8197 J-.0233
N390 X.82 Y0. I-.8187 J.0469
N400 G1 X.8203 Y.02
N410 X.8503 Z1.7
N420 X.85 Y0.
N430 G2 X-.85 I-.85 J0.
N440 X.85 I.85 J0.

[crazy^millman]

And just to vent for a minute, maybe I'm dense but what's the point of MasterCam treating my check surfaces as drive surfaces in all of the surface high speed cycles . I just want to tell the endmill not to hit some surrounding surfaces. but it insists on surfacing all my check surfaces. I have to use the old cycles to avoid this. How does that make any sense. Maybe I'm missing the point.

 

All HST toolpaths sorry not following you here. I use these toolpaths quite a bit and it I tell it a check surface no I do not see if machine it. Got a specific example so I can see what and where you are having such difficulty with these toolpaths?

[Colin Gilchrist]

I'm fairly certain we are addressing the Check Surface issue for the High Speed paths. I can't remember if this is for X8, or will make it into an earlier version, but I know it is being looked at. We do intend to treat Check Surfaces as "areas I want to avoid", instead of treating them as drive surfaces.

 

Thanks for the feedback Ray!

 

Regards,

 

Colin

[Guess_who]

Thanks for all the replies.

 

As far as arc outputs, when I've done simple flowline for chamfers in X6 it always produced arc. Doing the exact same thing in X7, does not produce arcs. The work around that I found was to check this box and set it to .010, then arcs are produced. Simple unchecking this box will give me a series of lines regardless of my setting for total tolerance. This makes no sense and seems to be backwards to me. I am surprised no one else is having this issue.

 

Here is the check box I'm talking about.

[Guess_who]

Crazy_millman, thanks for the example.

 

I think my filter settings must not have been allowing arc output. I am now able to get arcs buy just using the filter setting slider. Something I never really messed with before.

 

It makes sense to me now.

 

Thank you,

 

You guys are the bomb.

[crazy^millman]

Ray glad you got your brain around it. It took me a while to figure out what worked best, but as you can see the slider gives you a lot of control. For older machines I tell people set it one way and make that the defaults and for newer machines do it a different way and make that the defaults. Once set then you have it the way the machine likes and then yes you could forget ot even look here if you do run into problems.