[ChrisPhoenix]

All the tools in my library have a spindle speed of 5100 (I'm doing small stuff on a Tormach).

Almost all the time, I get the correct spindle speed and feed rate. But, occasionally, I'll have the correct tool but a spindle speed of 200. More occasionally, I'll have the correct spindle speed, but a feed rate of 200.

This is a great way to break tools - and even if I hit the emergency stop in time, it's a great way to waste time and metal (because there doesn't seem to be any way to go back a few steps on the Tormach controller, so I can't continue the job after interrupting it).

Is there any setting in SprutCam that will make it stop doing that????

Yes, I can go through all the operations right before I export, and make sure that the spindle speed and feed rate are correct. But the one time I forget...

Also, is there any way to make SprutCam assign the tool number from the library, rather than (apparently) setting them randomly? (I still haven't figured out its algorithm.) I'd like to have it stop for tool changes whenever I need a change, and not stop otherwise. If it would simply use the tool number that I assigned to the tool in the first place, this would be ideal. Otherwise, I have to set the number individually for each operation and then double-check.

Thanks,
Chris

[ChrisPhoenix]

I should say: When I create an operation, the first thing I do (if I haven't copied a previous operation) is select the tool from my library.

[Gerry Sweetland]

See the screen cap below... in the "Library selection" tab put a check in the box next to "Use tool number from library"
I'm not sure as I am not in the shop at the moment but if you are changing tool numbers after you set speeds and feeds SC will revert back to whatever the default was.
The screen cap was used in a previous post here on the SC forum for someone asking the same question about tool number. In addition if I remember correctly Tormach has tutorial that covers that as well.
Gerry

[ChrisPhoenix]

Gerry, thank you. Your quick answer has saved me hours of watching and re-watching the tutorial videos.

I'm currently working on an instructable to pass on basic tips like this, in text format which can be read quickly and navigated more easily than videos.

I'm wondering whether it's important to check the check box before or after hitting "apply"? This is the kind of thing that SprutCam often cares about and behaves ... counterintuitively ... when it's done the "wrong" way. (I would not have guessed that changing the tool number would _sometimes_ reset feeds and speeds to a number that's not in the library. That's very good to know. Thanks for that as well.)

Chris

[bevinp]

This is a great way to break tools - and even if I hit the emergency stop in time, it's a great way to waste time and metal (because there doesn't seem to be any way to go back a few steps on the Tormach controller, so I can't continue the job after interrupting it).

Two things:
1. Hitting the Emergency Stop button will stop all movement but there is no guarantee that the tool position will be exactly at the DRO position. If there was fast motion in any axis it may overrun the DRO position due to inertia. While the pause button is less sudden, Tormach advised me a few years ago that tool position may also be uncertain (this may have changed with the latest release of Mach3.

2. On one of the Mach3 screens there is a "Run from here" option (I am not in the workshop but I think the screen is behind the "Complicated"??? tab). This works well, but be very careful when using it. The tool is rapid moved from present position to a position indicated in the code line immediately before the selected line. It does this as a straight line, regardless of workpiece or fixtures. The positioning move seems more complicated if you have selected a code line just after a tool change. Practice using it without a tool in the spindle just to get confidence.

[ChrisPhoenix]

Ooh, Thing 1 is _very_ good to know. Thanks!

I found the "Run from here" option but I could not change where "Here" was. I wanted to go back a few lines...

Chris

[bevinp]

You scroll the code in the window until the line you want to run from is highlighted in the middle of the list.

[ChrisPhoenix]

I think I tried that, and the window always snapped back to the current line... I'll try it again. Thanks.

[bevinp]

Chris,
There is a known bug in "Run from here" that I have just experienced and emailed Tormach.

The bug is that if your program is machining by incrementing Z from a positive value downwards, and then select "Run from here", the pre-positioning movement will first rapid Z to 0, then rapid move X,Y to their positions nominated in the "Pre-positioning move" window that appears, then rapid Z to its nominated position, be it up or down. So if your workpiece surface is still above Z=0 and the current position of the tool is the other side of the workpiece, the tool will be driven rapidly into the workpiece.

But if your program starts cutting at Z=0, the "Run from here" works fine, assuming that the workpiece surface is below 0.

Tormach told me that ArtSoft will attempt to fix in the Mach4 release.

Tormach also told me that they (Tormach) advise not using "Run from here" or at least use with caution.

It is scary when you first use "Rfh" and see the tool rapidly moving over the workpiece. And guys want faster Rapids.... I'm happy with having at least a small chance of hitting the Emergency Stop button. I have the extension button fixed beside my keyboard.... it has saved me tools, parts, wear on the machine, and time wasted in recovery.

[ChrisPhoenix]

Ack, that would be pretty scary! I usually set my Z=0 to the highest flat on my part, to make it easy to zero in new tools. But not always... very good to know. Thanks!

[Moggot]

Is there a compelling reason to use 'Run From Here' over 'Set next line'?

I always use set next line. Just highlight or type in the line you want and hit set next line (just above the RFH button). The next time you hit cycle start, mach3 will start running from that line without any prep moves. So, obviously, it's helpful if you have the mill in a position where it can safely make the next command. I'll usually put the machine to it's tool change position and select the line preceding a tool change and/or new operation. It'll immediately ask me to change the tool and off we go, just like nothing had ever happened.

[ChrisPhoenix]

On the Tormach I'm using,
- Neither one works while a job is paused. I can't even scroll the GCode window. It took me a while to realize I had to rewind and start over.
- Both RunFromHere and SetNextLine would probably work just fine, when they work.
- The controller will scan through the GCode from the start to get to the start line.
- The controller sometimes wants to do a preparatory move.

[bevinp]

Chris,
After Pause is selected, selecting Stop passes control back to the user, and often the program scrolls down a lot of lines (don't know why it does this, perhaps it is the controller looking ahead). Selecting start will continue from where the pause occurs.

Must try the Set Next Line. Thanks Moggot