Question about 2D High speed Dynamic Mill toolpaths

[DavidSV]

Is there a way to force MC to have more clearance on the back feed part of the tool paths? Sometimes when I am clearing material the tool will hit the material on the back feed portion of the tool path. For example, if I am cutting steel at say 120 IPM feed rate, but with 250 IPM on the back feed, sometimes the crappier machines in the shop will hit on the back feed. I didn't know if there was a parameter or setting when I could tell MC how much space to put between the cut path and the back feed path.

 

Thanks

[gcode]

try setting your radius bigger

I have that problem with some of the big old dinosaurs we have here

[jeff]

I asked this question a few days ago,and the answer is no.

The only way to get it not to clip the stock on backfeed is to lower the back feedrate.

I have an Okuma 4020 MCV, and depending on the shape of the part I have to use 350 IPM or lower for my back feedrate.

I knew I should have got SuperNURBS on this thing when we bought it

[K2csq7]

I have an Okuma 4020 MCV, and depending on the shape of the part I have to use 350 IPM or lower for my back feedrate.

I have a big daewoo HMC, I use 30-50 IPM for the back feedrate and it still clips the corners!!!!!!

[jeff]

As Gcode said, make your radius bigger, but that doesn't help completely.

 

You could change your gap settings, and set your retract to "When exceeding a distance".

 

Or have a microlift amount larger than your depth of cut... this move is not a straight Z move.

[tedly]

You can keep Mastercam default setting only adjust your depth of cut. The most important to keep cutter from hitting stock is to draw stock on your cut geometries .1" wider on all cut sides.

[YoDoug®]

I asked this question a few days ago,and the answer is no.

The only way to get it not to clip the stock on backfeed is to lower the back feedrate.

I have an Okuma 4020 MCV, and depending on the shape of the part I have to use 350 IPM or lower for my back feedrate.

I knew I should have got SuperNURBS on this thing when we bought it

 

How old is the Okuma? It still should have Hi-cut even if you don't have super-nurbs. I program my tool path to leave around .03-.05 stock on the wall. Then I set my Hi-cut to .015-.03 tolerance and I have yet to clip a corner running up to 1000 IPM on my back feedrate. The mpmaster-okuma mill post has the functionality built in for turning on super/nurbs or Hi-cut with misc-reals.

 

G131 F1000. J1 E.01 (F=max feedrate, J=mode - 1 being high speed, E=tolerance)

.

.

.

G130

 

 

 

[jeff]

It's 5 yrs old, and yes it has Hi-Cut on it... but I always forget to use it because I'm not that familiar with it and don't really know how to tweak it.

You example shows a J, I don't think I've ever seen that before

What are the other types of modes?

[YoDoug®]

The modes available for Hi-cut are 1=standard or 2=high speed. I normally use 1 because our showroom machines don't get anchored down and with it set to high speed they start to move on us.

 

One other thing I forgot to add is in your MCX dynamic path if I set my stock to leave I always set my filter cut tolerance to slightly less than half of that and set it output arcs.Example, .025 stock gets a .01 cut tolerance. this make the tool path big smooth arc moves, combine that with proper Hi-cut settings and you get really fast moves that don't clip corners.

[jeff]

Thanks Doug, I'll definitely try that out.

I've only used it a couple of times in the 5 yrs we've had this machine.

[jeff]

ok in my Hi-Cut control parameters, my options are:

Hi-Cut control mode = Exist or Non-Exist

Max Feedrate

Tolerance.

 

When it says Exist or Non-Exist, does that allow me to use the J value in the G131? or is that simply saying that Hi-Cut is on?

 

I have the E100M control.

[YoDoug®]

In an E100M control the command is as follows. The E100M is an older version of control and the hi-cut is a different command than the newer ones.

 

G187 F1000. E.02 (F=max feedrate, E=tolerance)

.

.

.

.

G186

 

In the parameters when it says exist/none-exist that is the "all the time" Hi-cut settings. I normally have the parameter settings to have it on all the time and to a tight tolerance like .0002-.0004. Then I use the line command (G187 or G131) in my program to just open up the tolerance for high speed roughing only, then cancel the command (G186 or G131) to put the control back to tight tolerances for finishing.

[jeff]

Ok so if it's set to "Exist" all the time, it isn't actually ACTIVE unless I give it the G187 command right?

[YoDoug®]

I'm not sure in an E100M, I'll have to do some digging to find out, but in a newer control if it is set to exist/control on then it is active anytime the machine is in G01. When you use the G187/G131 commands it overides what is set in the parameters page with what is in the G187/G131 line of code. This allows you to change settings on the fly for different needs.

[jeff]

Thanks for all the info Doug, I've had it on for the past couple of hours, and it is active.

My cycle time went from 20 minutes to 28 minutes LOL!

Tolerance is set to .0003"

I

[YoDoug®]

Thanks for all the info Doug, I've had it on for the past couple of hours, and it is active.

My cycle time went from 20 minutes to 28 minutes LOL!

Tolerance is set to .0003"

I

 

 

Yep, that sounds about right. Use the G187 command in your program to loosen the tolerance as needed to improve your speed in roughing and leave it tight for finishing.

 

 

[Chris Rizzo]

fyi, X6 is reported to have better avoidance techniques. I'm experimenting with x5 vs. x6 right now to really check it out.