Multus B300 Thread Milling

[HooFan]

We have a Multus B300 I am trying to circle mill and thread mill the face of a part. I'm in top plane and right side views. When I post these tool paths the code comes out as line segments instead of arcs. Has anyone else had this problem and can you help? My tech guy says that the machine won't do it in arcs only line segments, but I've done it radially.

[Greg Williams]

Hi,

 

The machine will cut circles in G2/G3 XYZ arcs. They need to be broken at qaudrants.

[Columbo™]

in your control definition and in the arc page, check "support arcs in XY plane......see below

 

 

[Columbo™]

HooFan.....you have mail

[Greg Williams]

See if this works on your machine

 

G270 SP=1

M228

G270 SP=2

N0001 G140

N0002 G20 HP=4

N0003 G50 S2000

NA001

N0020 G20 HP=4

N0021 MT=00101

N0022 M321

N0023 M110

N0024 G94 M146 M15 M08

N0025 G20 HP=4

N0026 TL=001001 BA=45 G52 SB=3183 M241

N0027 G00 X121.214 Z10.607

N0028 G138 C0

N0029 G174 SX=50 SZ=0

N0030 G127 B45

N0031 G00 X0 Y0

N0032 G17

N0033 G00 C0

N0034 M13

N0035 Z15

N0036 G01 X-8 G41 F1273.2 M147

N0037 Z2

N0038 G03 X-8 Y0 Z0 I8 F254.6

N0039 X-8 Y0 Z-2 I8

N0040 X-8 Y0 Z-4 I8

N0041 X-8 Y0 Z-6 I8

N0042 X-8 Y0 Z-8 I8

N0043 X-8 Y0 Z-10 I8

N0044 X8 Y0 I8

N0045 X-8 Y0 I-8

N0046 X-6.096 Y-4.596 I6.5

N0047 G01 X0 Y0 G40

N0048 G00 Z15

N0049 Z15.001

N0050 G126

N0051 G175

N0052 G136

N0053 G95 M12 M146 M09

N0054 M109

N0055 G20 HP=4

N0056 M01

N0057 M02

[HooFan]

That looks great, now how do I get my post to punch out that code?

 

We just purchaces this post about 5 months ago yes I said 5 months ago and still have these issues. Could there be a evaluation setting on the post to not allow any changed to take effect not unless it is done by the company that it was purchase from? I tried e-mailing to and I was told there was a hasp lock of some sort on it as well.

[Columbo™]

who did you purchase it from???? was it in-house??

 

In-house WILL fix it to what you want, all you have to do is ask....

[Mick]

The output depends on what toolpath you choose, and what method (C axis or Y axis). That can be the difference between outputting drill cycles or not (as an example).

 

We have a Multus B400W, and we purchased the Inhouse post, and it works well. However, I do seem to recall some kind of problem with threadmilling ( I could be confused with the Mori Seiki MT post we also use though ).

 

I'll check out threadmilling using our post, and I will let you know.

[Matt Boozer from L&R PT]

Just so everybody knows who I am, I work with "HooFan" only on the mill side. We purchased it from InHouse. Not knocking the post by any means. I think there is a disconnect with the middle man ( our local dealer ) and that is what is frustating.

 

I think I read in here somewhere that we had to go through our dealer to get anything done with InHouse. Well, that is a problem because if we could just call InHouse directly and talk to somebody this would be fix and we would be on our way and not tring to find other people for advise.

 

When your tring to run a company and other outside people hold you up on getting issues resolved, not a good atmosphere to be in. We will give InHouse and CNC Software a call on Monday to see if we can get diconnect we are having reconnected.

[Mick]

I just trialled it. Using Y Axis, Right Tool plane, and the control definition set as per above in Columbo's post, the Threadmill toolpath output arcs.

 

Also, the arc did not need to be physically broken into quadrants for threadmill to output arc commands, but I am sure it needs to, to output arc commands for milling (I seem to recall having to do this)

[Matt Boozer from L&R PT]

we will take a look at again on Monday.

Thanks everybody again

[Greg Williams]

Helical G2 XYZ arcs do not need to be broken at quadrants but 2D XY arcs do need to be broken. To save the confusion It is easiest to break all arcs into quadrants. Gunguy please remember that this is a post setting. The actual geometry does not need to be broken into quadrants