OSP 300 Hi Cut can't turn it off

Captdave

Titanium

Joined

Sep 24, 2006

Location

Atlanta, GA

• Apr 14, 2016

• #1

We don't work with close tolerances very often so we generally only use High Cut when engraving part numbers and use G130 to cancel the cycle. Recently, for some unknown reason and I don't think anyone has messed with the parameters, Hi Cut is coming on with HSM roughing and severely slowing the feed rate. Have tried adding G130 at the beginning of the program and also before a HSM op and it still flashes and cuts the feed rate in some cases in half.

Anybody else have had this experience and if so how did you solve it?

 

X

XD341

Hot Rolled

Joined

Mar 23, 2011

Location

NY USA

• Apr 14, 2016

• #2

I leave hi-cut on all the time because most of what I'm doing requires decent tolerances. That being said I've only ever turned hi-cut on and off via the hi-cut parameters page. I was never able to get the g-code to function the way I thought it would so I just turned it on and left it.

I opened up the tolerances on the hi-cut parameters page and I haven't noticed any severe changes in commanded feed rate during HSM. Maybe I'm not pushing things like you are, I'm usually in carbon or stainless so my feeds might not be that high.

I've done some very nice surfacing in 6061 at 400 IPM and not seen a problem once I played with the hi-cut parameters.

 

Captdave

Titanium

Joined

Sep 24, 2006

Location

Atlanta, GA

• Apr 14, 2016

• #3

Any chance you could take a pic of your High Cut parameters?

 

T

TangentCNC

Aluminum

Joined

Feb 1, 2016

Location

Chandler, Az, USA

• Apr 14, 2016

• #4

Captdave said:

Any chance you could take a pic of your High Cut parameters?

Click to expand...

In your parameters you can turn it on to stay on all the time regardless of the Gcode. 100% its turned on in the system parameters. Check there first.

 

Captdave

Titanium

Joined

Sep 24, 2006

Location

Atlanta, GA

• Apr 14, 2016

• #5

TangentCNC said:

In your parameters you can turn it on to stay on all the time regardless of the Gcode. 100% its turned on in the system parameters. Check there first.

Click to expand...

I don't mind if its on all the time but I don't want it slowing down like it is now. Never adjusted it so I really not sure where to set it. If someone has a good setting then no reason to reinvent the wheel and I'll leave it on all the time.

 

Captdave

Titanium

Joined

Sep 24, 2006

Location

Atlanta, GA

• Apr 14, 2016

• #6

Took a quick peek and found 2 pages, high cut control and guide. Neither have edit fields so must not have found the correct page.

 

Mtndew

Diamond

Joined

Jun 7, 2012

Location

Michigan

• Apr 15, 2016

• #7

It's called Hi Cut Pro Control parameter.
It's right around page 33 or 35 on the parameters page depending on how many you have set to be visible.
I keep ours set to "Standard" and about a .002/.003 tolerance.
If you have it set too tight, it will bog down the feeds in corners for sure.

After you change the settings make sure you hit the "Para update" softkey.
If you change it while running a program it will change when it hits a G00, or after the read-ahead completes its buffer.

 

X

XD341

Hot Rolled

Joined

Mar 23, 2011

Location

NY USA

• Apr 15, 2016

• #8

Para menu 36 (on mine)

Hi-cut Pro parameters

on in control
upper limit 500 ipm
tolerance .003
mode: High Speed

I used that for making a really nice surface in 6061 at 11k and 400ipm with a 5/8 ball. It was an automotive part and the total profile accuracy wasn't that critical. It fit air...lots and lots of air. Not overloading the tool was critical for finish reasons and those settings worked nicely. It slowed down only in the tighter radius where the machine was switching direction. The rest of the cut was right at 400ipm commanded.

 

Captdave

Titanium

Joined

Sep 24, 2006

Location

Atlanta, GA

• Apr 15, 2016

• #9

Ok found the right page and made the adjustments.

Thanks for the tip on the obscure "save" button, I'm sure I would have over looked that one.