[Arnoldjrimmer]

I'm just getting started with a Dolphin and Mach 3 lathe set up but I have a small problem with the tool select command.

When I run the post processor I get something like:

N60 ( Standard Turning Tool )
N70 M06 T1 G43 H1

Mach 3 doesn't seem to recognise T1 as a tool change command. If I manually change it to T0101 (or T0201, or whatever) then it works as it should.
Shouldn't the post processor (I'm using T_Mach3Rcss.ppx for radius mode) output the tool number and offset number in the code? Or am I missing something.

Any help with this would be greatly appreciated as I've spent the last three hours trying to find a solution on my own.

[andre-dolphin]

Hello,

Strange how this hasn't been an issue before, I wonder if it's something to do with the MACH setup on your PC.

We can easily change the post if that is required, perhaps one of the MACH3 gurus here can shed any light on this.

ATB
Andre

[Hood]

Mach Turn requires the tool call in the T**** format and any post processor I have used with Dolphin Turn has used that.
In the very early days of Mach 2 Turn then I think the M6T* but that was a long time ago, probably 7 or more years.

Hood

[LeeWay]

Hood is the Man!
It does sound like the post is not outputting what you need. Hood is the guy that reined in my PP to work with Dolphin and I get exactly what I expect every time now. Lots of different ways to setup and run a lathe. It is great when you have a post that is adjusted correctly for what you need. You have to know what and how to change things and after working on mine with Hood, I dove in and can now change a couple parameters in a PP.

Open one up and have a look around in it. If you change anything at all, change the name too. You have to be careful with them, but they are easily edited.

[Arnoldjrimmer]

Thank you for the replies.

I found another post processor on a forum somewhere that appears to use the correct tool change code. I think that the other tool change code was in fact working; it just wasn't updating the tool DRO on Mach3.

I don't understand why I, or anyone, would need to have a different post processor. Surely, if it is right, then it is right. How can I be the only one to have this problem when I just used the post processor on the Dolphin website?

I have been having all sorts of other trouble though. I have been able to run simple programs without a problem so I think that my Mach 3 set up must be okay, but when I try anything more complicated, the programs have been running the tool into the workpiece half way through. The simulation looks fine in Partmaster CAM so I don't know what's going on.

I'm now trying to create another program that uses 2 tools (turning and boring) but I keep getting the message (seemingly at random) "The finished part profile has been reduced to a single line. It is not suitable for this operation" with my boring operations. I am trying to turn the bore in 2 parts so that the operations don't create too much swarf and clog the hole. I can't figure out why I get this sometimes and sometimes not.

There seems to be no reference to this in any of the documentation that I can find.

[andre-dolphin]

Can you upload the file in question to the files section here and I will take a look at it.

ATB
Andre

[Arnoldjrimmer]

I managed to do the machining with doing the boring operation in one hit. It worked okay but I was worried that my (rather expensive and fragile) carbide boring tool would break if the hole was overloaded with swarf but I just made sure to brush the swarf off the tool between each pass. Unfortunately, I don't have the program any more for you to see. I still have the G-code, if that would be any use to you. I would still like to find out what the problem was so I know how to handle it the next time. If I can find the time I will try to recreate the problem on a new program so that you could take a look.

I think all of my toolchanging problems are solved now with using the other post processor and having a better understanding of how Mach 3 deals with tool offsets.

Anyway, I have another problem which it that when I create a program with any boring operation and have the "roll sharp corners" box checked, Mach 3 cuts inverse arcs at each corner. I can fix this by changing the "IJ mode" but then the outside turning corners and radii have inverse arcs. I have been able to run programs successfully by unchecking the "roll sharp corners" box but if this means that I can't create a program that has internal and external radii and have both of them machined correctly. Is there anything I can do to fix this or is it something that needs to be changed in the post processor?

My set up is a slant-bed lathe with the toolpost on the rear of the spindle axis. The machine is set up so that X negative is away from the centreline (so X -2 cuts a 4mm diameter). Is there any problem with running like this? I have it like this because if I have X positive away from the centreline jogging in Mach 3 is inverted because the 'up' key would move the toolpost down as I see it.

[Hood]

First thing I need to ask is what version of Dolphin are you using, 10 or 11?

Why do you have the tools set up backwards like that? X Positive should be when the tool is moving away from the centreline and thus cutting a larger dia, you can change the jog direction of the keys to what you want in Mach.
I have two lathes, one a large lathe with a rear turret the other a small with a front toolpost, both are set up so that a jog out on the X is moving positive. Wee lathe that means jog positive and the tool moves towards me as it is a front post lathe. Jog positive on the big lathe and the tool moves away from me as it is a rear turret lathe.


Hood

[Arnoldjrimmer]

I'm using Dolphin version 10.

With the set up as I have it, the toolpath display on Mach 3 shows the tool as coming from the rear of the work (as I see it), when I tried changing to a non-inverted X axis, even with the tools set as being in the rear toolpost in the tool table, the toolpath display shows as approaching from the front of the work. This, in addition to not knowing it was possible to change the jogging key designations in Mach3 is the reason why it is as it is.

Do you think that this could be a solution to my problems, or is it just best practice to have it set up in this way? It would make the machine more intuitive to use. Is there a way to have the machine set to use positive X as you suggest but to have the toolpath show an approach from the rear?

Thanks for everyone's input with dealing with my troubles, I really appreciate it (I'll be VERY happy if I can get the machine and software working perfectly).

[Hood]

Ok , I thought that may be the version you are using. There was a bug in Rev10 that reversed the arcs for internal tools. If I recall correctly the way I got round that was by telling Dolphin the boring tool was actually a front tool approaching from the rear. Doing that and the code produced would be good, the simulation in Dolphin would show the tools as front but the code would be fine.

Yes Mach can display tools above centre no problem, hopefully I have managed to attach two screenshots, both are the same file but one is loaded into the big lathes profile, the other the small lathes profile.

There are quite a few settings in Mach that can affect things and really the easiest way would be to see your xml, not sure if you can attach them here, if not the Mach forum may be the place to go.
General Mach Discussion

Or maybe you could pm me and I will let you know my email address so that you can forward your xml.
Hood

[Lasersolution]

wow, we are factory of cnc router and laser cutter, with can give you help in futhure