New Onecnc user!!

[wms]

Smitty,

Look at the second page of your nc setup and make sure the scale factor is set to one as shown.

If this were set to 2 in x then it would double your x code.

But looking at the code you posted, it looks right, so I doubt this is not set to 1.

[smitty]

HMMM,
Well at least it works on your machine, that's good news.
Default is absolute in Turbocnc, I'm not to sure on the radius VS diameter programming, I will check on that.
Thanks for the help, Time to put the Kids to bed and think about this a little more.
I'll keep you posted!
Smitty

[smitty]

WE HAVE CHIPS!!!!!!
If I knew how to do a back flip, I'd be all over the place!!!
I removed the diameter cutting, set me zeros, and by george, we have a dogbone!!!!!
I can't thank you both enough! WMS and HFD, could not have done this with out you!!!!! I was just about to give up, now I see the light, it may be dim, but I can see it!
THanks again,
Smitty

[HuFlungDung]

That is great news, Smitty!

Now you can settle in for some less stressful learning

Does Turbocnc allow you any option for diameter programming? I always found it more convenient to program diameters, because that's what my micrometers read: diameters.

You might even be able to change a scaling parameter in your Turbocnc so you can input diameter values. Just "lie" to it about what your screw thread ratio is

[smitty]

The first step always seem to be the hardest! But once it is done, it all seems to flow.
As for diameter turning, that I will have to look into.
Thanks again for the help, I am off to the real world now.
Smitty

[dkowalcz]

Originally posted by HuFlungDung

Does Turbocnc allow you any option for diameter programming? I always found it more convenient to program diameters, because that's what my micrometers read: diameters.

You might even be able to change a scaling parameter in your Turbocnc so you can input diameter values. Just "lie" to it about what your screw thread ratio is

Hu:

Yes, but it's sort of a hidden feature at present. Needs a hand edit to the ini file to make it kick in. I learned radius programming originally on lathes and didn't add it to Turbo until recently - about a year ago.

Lying about the thread pitch works well too, as long as you don't use G02/03.

-Dave
Author of TurboCNC

[smitty]

Hey Dave,
You made it!
Just finished making a part out of Delrin, although it looks close to the design, it is different.
Should I consider another tool for the final finish pass. I am using a .040 wide tool, with a full radius on the end.
Thanks for all the help guys!!!
Smitty

[smitty]

And yes there are more questions!
When I go to set up my tools, are the dimensions for the tools all in metric, and does that also apply to the diameter of the material?

[wms]

Smitty,
The box you are looking at only aplies to the simulation, not the tool setup for generating code. But you probably knew that.

The tool is metric and all the rest ( diameter ect.) are Imperial, (if you are using imperial.)

And don't ask me why the tool is metric....because I don't have a clue.

[smitty]

Thanks WMS,
Just thought I would ask. It got me wondering, because it comes up after the code is generated. Now I know!
Smitty

[dkowalcz]

Originally posted by smitty
Hey Dave,
You made it!
Just finished making a part out of Delrin, although it looks close to the design, it is different.
Should I consider another tool for the final finish pass. I am using a .040 wide tool, with a full radius on the end.
Thanks for all the help guys!!!
Smitty

Hi Todd.

Well, ordinarily I like to use the same tool for rough and finish - a toolchange for that is sort of academic on a benchtop machine. Takes too much time away from the primary goal of making scrap besides.

Sure that part doesn't need support? Seems a bit long to make out of delrin all in one setup.

I guess we're getting a bit off topic for the forum here...

-DK

[HuFlungDung]

Originally posted by smitty
Hey Dave,
You made it!
Just finished making a part out of Delrin, although it looks close to the design, it is different.
Should I consider another tool for the final finish pass. I am using a .040 wide tool, with a full radius on the end.
Thanks for all the help guys!!!
Smitty

Hi Smitty,

Describe the differences you see. Is it just part flexure?

You may be getting into the area of tool nose radius compensation.

How would you tell? Well, typically you would have already been making adjustments to your tool offsets until the measured diameters are correct, however, the ball ends would appear to be compressed or stretched in the Z direction, because the cutter is overcutting or not cutting it enough.

Let us know, so then we can discuss the correct issues.

[smitty]

Dave,
I was using Delrin just to test how things where going to work. HFD, you are right about the balls, they seemed squished in the center, I do not think Turbocnc has cutter comp.
When I mounted some Titanium and ran the program, the shaft is .030 to thick, and the final pass never touched the material.
I just finshed re-loading my PC, so I need to re-load Onecnc as well and re-do the program.
I hope to be back on this tonight or tommorrow.
Thanks for the help as always!
Smitty

[HuFlungDung]

Not to worry, Smitty, your controller doesn't need to be able to do cutter radius compensation, because you can do it within Onecnc and get correct results.

You need to think of your tool reference point (TRP) as being located at the center of the nose radius. This means that the tool material actually projects outwards from here by the amount of the radius.
So, if you were to force the TRP to follow the exact profile that you drew, then the part would be too small, by the amount of the tool radius (*2= diameter).

Thus you need to create an offset profile to make allowance for this tool radius. But, don't draw an offset, let Onecnc's finishing cut routines do it for you, that's what they are there for.

When using the Onecnc lathe roughing and finishing routines, tool nose radius is already accounted for if you specified a proper tool radius in your tool setup.

Since the compensated path is away from the lathe axis and away from the chuck, your X and Z tool offsets should be adjusted in the respective opposite directions.

If one finish pass is too much material to remove, then you can opt for more than one, of course.

[dkowalcz]

Originally posted by smitty
Dave,
I do not think Turbocnc has cutter comp.
Smitty

You're right. It doesn't, yet...

[smitty]

Thanks,
I hope to have things running again later tonight, and give it another whirl!
I am optomistic to say the least, when I make these parts manually, it takes me an hour for only one,.... 7 min. using Onecnc!!!
Was I happy? Understatement!!!!
Smitty

[smitty]

I am REAL close to the real thing now!!
Just a couple more questions,
I have just finished turning a piece of Ti, and the X is only moving half the distance needed. In other words, the shaft diameter needs to be .170, and right now it is at .233.
So, I am assuming that the Dimensional turning in the NC post needs to be on, but that will cause my X axis to move away from the material to far, like before.
So, that brings me to Mr. Dave at Turbocnc!!!
How do I turn on the Dimensional turning within Turbocnc?
I also stopped using the grooving cycle, as I like the one tool option instead, takes a couple mins. more, but not a problem.
Thanks for all the help, Just about gave up on this!!
Smitty

[HuFlungDung]

Smitty, do you mean "diameter turning" instead of radius?

[dkowalcz]

Originally posted by smitty
So, that brings me to Mr. Dave at Turbocnc!!!
How do I turn on the Dimensional turning within Turbocnc?
I also stopped using the grooving cycle, as I like the one tool option instead, takes a couple mins. more, but not a problem.
Thanks for all the help, Just about gave up on this!!
Smitty

Easy.

Edit your turbocnc.ini file with a text editor like Dos's EDIT command or NotePad in windows.

Change the line that reads:

ABSprescale=1.000

to

ABSprescale=0.5000

for the X axis only. All absolute moves will then be divided by two internally, and incremental moves left in actual units - which makes everything work properly on a diameter programmed lathe, assuming you zero the tools at the centerline.

Depending on which version of Turbo you're running, the values in the ini file might be in scientific notation:

1.0e+0000 is the same as 1.00

5.0e-0001 is the same as 0.50

Just input 0.500, the computer doesn't care and it's a lot easier for most folks to think in radix point.

Good luck. I'll have to drop by your place again sometime and see what you're making.

[smitty]

Come on DOWN!! You are more than welcome.
Basicly, I am making the same stuff, but NOW with CAD/CAM!!
What a learning curve, but it is good to teach old PUPS new tricks, thats what the wife says!!!
I will give that a try and see what I come up with, closed eyes and all!
HFD, yes you are right, Diameter turning. I got excited again, I am so close!!!!
Smitty