[Martin 007]

It decided to take a short cut.....


N5105 M00
/ ( /FEATURE POCKET HIGH SPEED)
N5106 M08
N5107 G90 Z0.1
N5108 X-0.1101 Y1.381
N5109 S2360 M03
N5110 G01 Z-0.436 F9.4
N5111 X-0.3544 Y1.328
N5112 G17 G03 X-0.0571 Y1.1367 I0.2443 J0.053
N5113 G02 X0.2452 Y0.9846 I0.0571 J-0.2631
N5114 X0.2693 Y0.873 I-0.2467 J-0

[neilw20]

That's what you call a leadin/leadout!!
Did you run it in an emulator before cutting chips?

[Martin 007]

The code I copied from Preditor Editor.... I just didn't see it when I back plotted it. I haven't fixed the preditor yet so I cant see the part.... I just see green lines... and lots of them. The other pic is from Bob and is the tool path that it generated.... The high speed pocketing did a few other weird things as well.... I will just have to go back and review it all.... think I will fix the software first....

[jrmach]

Oh my Martin.
First thought is it a pp problem.But then again not all that sure.HSP can do bad things when inputs or geometry not good.You need to get Preditor working right.If you see it gouging in Preditor I would change your leads to Verticle.
If you want to load the file you ran and PP we can have a look.

[Martin 007]

I deleted it.... The Geo is clean.... i think it is the HSP doing it.... It also did some wiered tool path.... Sudden increase in feed to clean off little bits.... and some just plain stupid stuff... probably needs a upgrade as it is at least a year or more old. Anyway I'm machining basic stuff for a job.. and that is going well, so I don't want to go futzazin with it yet.....LOL
Will verticle plung the bit.... I try to stay away from that.... One of the issues.... it sat there and did the ramp circles.... like 4 of them.... Z never moved.... then bam straight dow and go like it had pre cut the ramp... Anyway.. I'll get back a bit later.....

[Martin 007]

Here is the file.... as it stands now....

[jrmach]

Check this out,just to give you some ideas of settings.Note I did not set speeds and feeds,I can if you would like.Note on HSP you set feeds any where from %25 to %75 higher than other tool paths.That more than makes up for what appears to be wasted moves.A lot of those moves that appear to be unnecessary are all about how the cutter enters and executes it cut.Easier on the cutter with a constant load.Hence you can really crank up the feed.
I don't know if you quite got what I said in previous post so I say again,Ramp is what is supported for the material entry.That is why you see all those paths going round and round.Check out all the settings I chose and you will see a noticeable difference that what you chose I suspect.They all play an important role on the tool path.The one I did has probably 1/4 the total inches traveled as your earlier ones.I might add that if was me I probably chose a slightly different tool path strategy,but this works too.

[Martin 007]

The two big changes.... is the 70% of cutter... and aproach angle of 10K over 3K...
I will play with it and see what changing up....
the tool changes at this point is a pain... as I don't have the offsets setup.... therfore I have to get it back to a zero top of part.... using the foot lift....
Thanks for going to the effort... I have a few tool pathss left and then I'm going to go to the download they sent me to fix the Prediter and such.....

[mactec54]

Martin 007

Was this right at the end of the program, when it had finished cutting the part

[Martin 007]

No it was the first thing it did in the finishing pass....

[Martin 007]

Well now I need to watch feeds.... Different part... i checked everything else.... all good.... It set the rpm at 1431 and the ramp feed was 11.5 Then it went to 22.3 still at 1431 rpm.... For sale.... 7/16 4 flute short end mill.... Time to do the repair on this software... All is good ... Happy New year.... Be safe.... I'll return after the repair....

[mactec54]

Martin 007
No it was the first thing it did in the finishing pass....

Just look at the program, to see if it has a G0 X Y Z move on the same line at the start of the finishing pass

Or if the code you have above, will cause a crash to, as you have a G1 -Z then a X & Y move this may crash if the Z is down & the X & Y are moving to a position

you need to have the X & Y move Before the G1-Z move if this is the case

The G17 should not be in the G-code program were it is as well, should only be at the begining of a program, in the safty line

[Martin 007]

Thanks mactec... I'll look into it and compare with the repaired version... Which I can easaly see has changed.... New toolpath has a feed # on almost every line... Speeds are in line with rates. It didn't however fix the prediter editor and VPE... oh well still works enough to search code etc....

[Martin 007]

mactec.... It's up on the first post.... it put a g90 and z.1 which is the clearence...

[Martin 007]

Ok maybe someone can help with this one. Feed speed is way wrong and to my knowledge I haven’t changed any system settings to make it that way. On a regular pocket it did the same thing. Ramp into material pretty normal and then went to 22 without changing the spindle RPM.
Here is the known data for my calc and BC’s…. ( .4375/4 tooth and aluminum.) I gave mine a 280 SFM and spindle speed should be +/- 2400 and feed rate of 29…. BC came up with 1431 rpm and feed rate of 22. My calc at 1431 comes to 17. The 11.5 Z feed BC came up with seems more in line to me.
So how can I fix the way BC throws this in there…. I don’t want to edit feeds/speed for every file or for that matter… line….
Here is the top of the depth circles and then I’ll put the bottom part….
/ ( /INNER 7/16 4)
N01 M08
N02 G00 G90 Z0.1
N03 X0.0124 Y-0.0015
N04 S1431 M03
N05 G01 Z-0.0001 F11.5
N06 Y0.0017 Z-0.0003
N07 X0.0115 Y0.0049 Z-0.0005
N08 X0.0099 Y0.0077 Z-0.0007
N09 X0.0075 Y0.01 Z-0.0009
N10 X0.0047 Y0.0116 Z-0.0011
BOTTOM OF CIRCLES…..
N78 X0.1576 Y-0.1693 Z-0.099
N79 X0.1762 Y-0.1498 Z-0.1006
N80 X0.1924 Y-0.1283 Z-0.1023
N81 X0.206 Y-0.1051 Z-0.104
N82 X0.2168 Y-0.0805 Z-0.1057
N83 X0.2247 Y-0.0548 Z-0.1073
N84 X0.2295 Y-0.0284 Z-0.109
N85 G17 G02 X0.2295 Y-0.0284 I-0.2295 J0.0284 F22.3
N86 G01 X0.0124 Y-0.0015
N87 G02 X0.0124 Y-0.0015 I-0.0124 J0.0015
N88 G00 Z0.1
N89 Z-0.0091
N90 G01 Z-0.1091 F11.5
N91 Y0.0017 Z-0.1093
N92 X0.0115 Y0.0049 Z-0.1095
N93 X0.0099 Y0.0077 Z-0.1097
N94 X0.0075 Y0.01 Z-0.1099
On a separate note… If I can change the way BobCad default calculates feed rates… I would like to change the arc slowdown from 100%. I think it is a little slow… Not sure what a good rate would be. But again on a default basis….
Thanks... hope all of you are having a great day so far!!!