[usarty1]

Hello Men,

So far the PNC 1100 Has been great! I want to wish all of you a blessed holiday season and great Christmas.

Here is my question, I was milling a pretty expensive part and found the need to change the code to correct a problem. I kept the part in the fixture and retained X,Y and Z. I cannot seem to figure out how to start the machine up at a line number in the G code to avoid having to start completely over. The part takes 13 hours to fully cut! I cannot seem to find or figure out how to call the line number for a tool and start cutting again from that point. As always your help is greatly appreciated. I will be posting some cool three D parts once I can get through this road block and not waste the stock.

Kind Regards,
John
USMC Retired

[LRF]

I have also wondered the same, so here is an idea. Copy the GCode and give it a new name so you don't lose the original. Now edit the code as loaded and delete all the code already ran and then start the code where you need to.
Then on the next new piece reload the orginal code and away you go.

Just an idea, I have never yet had to do this but would be my plan till I figure out the right way, if there is one.

[usarty1]

Thanks LRF,

I am reading the manual section 5:10 and the screen does have a line start option but still not sure it will work by just typing in the line. I just did what you sugested but it is a bit of a time consuming hassel but does work. Evdently there is a way to do it, therefore I am going to keep reading. Hopefully someone has used the option Run From Here in the software screen slection. It is some what covered in 5:10 of the PNC 1100 Manual.

Thank you and Kind Regards,
John

[jid2]

If the tormach version is the same as regular mach...

Scroll through the code in the mach 3 interface, when you find your spot hit the "set next line" button. Make sure the reset is live. From there it's just "cycle start".

You need to make sure the machine is in a good spot given where the code is going to take it.

Run from here does crazy stuff.

[usarty1]

Thank you Jid2,

I would only try once it finished the tool path for the tool and has returned to zero. I am going to give it a shot and to be safe run in the air first. Sounds simple enough and greatly appreciated sure will save me 12 hours.

Merry Christmas and Thank you,
Kind Regards,
John USMC Retired

[IMT]

I use the "Run From Here" all the time. Your situation is exactly what it is intended for. *Just move to the line of code where you want to start. Pick the line carefully, you want to choose one where the tool is above the workpiece on the Previous move.
*Then hit "Run From Here" and it will simulate running through the program up to the chosen start line without actually moving anything. This may take awhile if you have 1000s of lines of code.
*Then it will tell you to "press cycle start to see the preperation move". A window will pop up telling you the xyz coordinates of where it will move to. NOTICE the RAPID HEIGHT value which defaults to 0. You need to change this to a value large enough to put the tool above the workpiece and fixture. It will first move Z to the rapid height, then to the target xy, then to the target z. There is also an option to turn on the spindle before moving. Use this if there is not an S3 command in your code following you starting line.
*Then press OK. It WILL MOVE as soon as you hit OK in the window.
*After it completes the prep move it will prompt you to "hit cycle start to begin" and you're off and running.

[usarty1]

Thanks for the info IMT, Can you tell me if you choose a line that a tool change is required do you still need to go through all these steps or can you cycle right from that line with the tool change if the tool is moved off the part?

Kind Regards,
John USMC Retired

[usarty1]

This is part that I have been working on, 3D from a photo of the Boston Light for one of our family Businesses. This part is hundreds of lines in the code, one of the reasons I may need to run from a line in the code if something needs to be tweaked. The final cut for detail is a .062 Ball end mill, total run time 13 hours for one part. Deferent versions and stages of production.








Kind Regards,
John
USMC Retired

[LRF]

Very nice!
A couple questions if I may, what software did you use in converting the photo to 3D and then what CAM software did you use please?
What is the material you used?

Thanks, Lynn

[IMT]

Thanks for the info IMT, Can you tell me if you choose a line that a tool change is required do you still need to go through all these steps or can you cycle right from that line with the tool change if the tool is moved off the part?

Kind Regards,
John USMC Retired

Actually in 2.5 years with my 1100 I have always used "run from here". I suppose that would work if all the parameters were still set and your not using any variables that need to be set. Try it and let me know how it works.

-Dan

[Steve Seebold]

This part is hundreds of lines in the code, one of the reasons I may need to run from a line in the code if something needs to be tweaked.




Kind Regards,
John
USMC Retired

Sir, I think you are mistaken. Hundreds of lines of code is a very inaccurate estimate. I think it's more like THOUSANDS of lines.

Anyway, that's "beautiful". What software did you use to generate the code?

[jid2]

Nice Part!

And thanks IMT for the detailed description of run from here. I missed the Z rapid height set at zero by default - that was the problem I've had with it!

[dbrija]

Very nice!
A couple questions if I may, what software did you use in converting the photo to 3D and then what CAM software did you use please?
What is the material you used?

Thanks, Lynn

PhotoVcarve does this nicely (both the photo conversion and the CAM). You just have to make a few edits for starting the spindle, etc... and let her rip (for hours and hours.....). Oh to have a 15-20k spindle....

[usarty1]

Very nice!
A couple questions if I may, what software did you use in converting the photo to 3D and then what CAM software did you use please?
What is the material you used?

Thanks, Lynn

Hi Lynn,

I use BobCad 25 with Bob Art, if you use the software just make sure you check the G code, it works best going from the larger size End Mills down to the .062 Ball to get the super fine Detail.
Kind Regards,
John
USMC Retired

[shred]

I use run-from here too, but the prep moves are stupid and it's real easy to crash at that point (even easier with the ATC, although it tries hard to do the right thing), so either do the preps without a tool in the spindle or edit the Z. With the shuttle, you can also move Z around even though the keyboard is blocked by some dialog.

[SCzEngrgGroup]

If the tormach version is the same as regular mach...

Scroll through the code in the mach 3 interface, when you find your spot hit the "set next line" button. Make sure the reset is live. From there it's just "cycle start".

You need to make sure the machine is in a good spot given where the code is going to take it.

Run from here does crazy stuff.

This works, sometimes better than "Run From Here", which does do STUPID things at times.

HOWEVER, if you use "Set Next Line", Mach3 does NO setup before starting to run from that line. If, for example, the code expects the spindle and coolant to already be on at that point, it WILL NOT turn them on for you. You have to do that before hitting Cycle Start. So, basically, it is up to you to ensure the machine is positioned correctly to execute from the chosen line, and that all offsets and modals are properly set, or you won't like the result.

Regards,
Ray L.