How would you do this?

[wbleeker]

I have a job to do that is 6061 aluminium flat 10mmx20mm x 92.5 mm, I have machined the pieces to length ( there are 30) I have to drill 5 holes through one face,two in each edge and one in the end. I have got the program worked out to do the five holes.
How I was going to do the job was to do a separate program for eace face, but thought maybe I could do it all in one program, with stops in between faces?
For the end holes I was going to put five pieces together side by side.
Any advice or suggestions will be appreciated.
Will

[wbleeker]

I just tried to do another program for two of the side holes and even though I reopened the IGES file it is not letting me move the co ordinates to the top of the next surface? i know I am probably missing something, but that is what this forum is for for isn't it? Thanks for any help
Will

[TXFred]

You'll need to add additional work offsets for each operation. Next to the pulldown menu at the top of the screen (Probably says "Global CS" right now) is a blank sheet of paper. Click that, and you can create a second coordinate system. Assign that coordinate system to G55, assuming that your first CS is G54. Enter the rotation values and offsets needed to put the new origin in the right spot. You can go back and change the offsets later, but once you enter the rotation value, you cannot change it without deleting the new coordinate system.

Then, when you create additional operations, you need to set those operations to use the new coordinate system for the Workpiece Setup, Workpiece CS, and Local CS.

You can program all of your operations in a single SprutCAM file, and when you post them, you will get one program to do everything. If you need to have separate programs, you will have to break the program apart by hand. This is pretty easy to do in a text editor.

Save a copy of your file before you start. You'll likely mess something up the first time, so you want to have a good copy to go back to if this happens.

Frederic

[wbleeker]

Thanks Fred
If I do the program as you suggest, will the machine stop once it has performed all the operations in each coordinate system, to allow turning the workpiece for the next operation? and if so then could I just put in a new workpiece and rerun the same bit of program- in essence then I would only have one setup for each side but could run any number of parts.
Will

[TXFred]

Thanks Fred
If I do the program as you suggest, will the machine stop once it has performed all the operations in each coordinate system, to allow turning the workpiece for the next operation? and if so then could I just put in a new workpiece and rerun the same bit of program- in essence then I would only have one setup for each side but could run any number of parts.
Will

No. It will attempt to run the entire program. That's why you might need to break up the program into multiple parts in a text editor.

If you're doing a large number of parts and have room on your table for multiple fixtures, this can work to your advantage. Set up a fixture for each operation, and you can get an assembly line going.

If you do this, you will want to reorder your operations to eliminate unnecessary tool changes and table movement. Suppose that Op 1 drills a 1/8" hole, and then chamfers it. Op 2 also drills a 1/8" hole on a different side of the part, counter bores it with a 1/4" end mill, and then chamfers the counterbore. Op 3 uses the 1/4" end mill to cut a pocket, and then chamfers the pocket.

If you do all of that in the order I just listed, you would have to make seven tool changes. If you reorder it, you get this.

Change to 1/8" Drill
Op 1 drilling
Op 2 drilling
Change to 1/4" End Mill
Op 2 counter boring
Op 3 pocketing
Change to Chamfer Mill
Op 3 Chamfering
Op 2 Chamfering
Op 1 Chamfering

Now you only have three tool changes per cycle. Also, the mill spends as little time as possible moving between the various fixtures. With the Tormach's slow rapids, that will add up to a lot of time saved on a high volume job.

The other scenario is where you have a single fixture that is used for all three operations. For instance, if you have a single vise that will do all the work holding. In that case, you definitely want to break up the program. Run Op 1 on all of your parts. Then run Op 2 on all the parts. Then run Op 3. If you try to run Op 1, then Op 2, then Op 3, on a single part, and then do the same for the next part, and the next, you're eventually going to get confused and load a part incorrectly. The result is broken tooling and a ruined part. You're better off keeping things simple.

This is more than you asked for, but once I get typing, I find it hard to stop.

Frederic

[wbleeker]

Fred
Thankyou very much for putting in the effort to reply, I really appreciate it!
As far as simplicity goes, how about if I do one program for one side and then Post Process it and re-open the IGES file and do the next side?
Let me know what you think.
Will

[MichaelHenry]

You could also insert an "M0" (number zero) after each op. That will pause the program until you press "Cycle Start". Watch out for your offsets, though.

I think Eric from SprutCAMAmerica did a tutorial video on how this can be done from within SprutCAM. You can find those on YouTube.

Mike

[TXFred]

Fred
Thankyou very much for putting in the effort to reply, I really appreciate it!
As far as simplicity goes, how about if I do one program for one side and then Post Process it and re-open the IGES file and do the next side?
Let me know what you think.
Will

You can do it that way, but it's going to be more work, especially as your parts grow in complexity.

Frederic

[wbleeker]

Thanks again everyone, I am a bit short of time at the moment, so rather than try and do a complex program I will probably do it in bits. I only have ten days until we are off on holidays for a month and with running our normal business as well as learning CNC and Sprutcam I will stick with the KISS method this time.
Thanks
Will

[slowlearner]

Call me stupid but please tell me what justifies holidays for a month? Is it a paid holiday? I am a foundry patternmaker by trade, is there any demand in your country?

[wbleeker]

Call me stupid but please tell me what justifies holidays for a month? Is it a paid holiday? I am a foundry patternmaker by trade, is there any demand in your country?

Owning our own business that operates 12 hours a day,7 days a week, 364 days a year! Yes we paid for it! We make and sell Pies if you google you will find our business, we don't have a website our business name is "The Famous Robertson Pie Shop" you might have to select pages from Australia, if you have seen the movie Babe it was made here.
I don't think there is much demand for a Foundry/Patternmaker here but am not sure, I know there is a massive demand for people to work in the mines as we are experiencing a mining boom.
By the way I just realised a lot of you don't get paid annual leave? I think that is right, all Australians in full time employment get at least four weeks paid annual leave a year at their same pay rate plus 17.5%, which usually cuts out their income tax on their pay.
Will