Does anyone here use SC 12 for the Tormach lathe?
I've been having problems with transposing the part to the correct orientation, the tool library and a few other things.
Printable View
Does anyone here use SC 12 for the Tormach lathe?
I've been having problems with transposing the part to the correct orientation, the tool library and a few other things.
Hi Mike,Quote:
Originally Posted by MichaelHenry
Did you get this working for you?
I use sc14 and currently working thru setting up some programs using the lathe module.
From what I see it looks like you can setup parts almost automatically after you get the tool orientation and approaches set correctly.
And of course the tools defined accurately in tool table.
I can get some decent tool paths with approach from a turret or above part. So far I get strange errors on any tool approach from below or in front of part.
Anyway 1 will be working in lathe module a little and maybe we can get others interested.
Learning curve on cam programs can be down right frustrating and I can use all the help and pointers I can get
Looks like this works pretty well. I have no clue how it wants me to create tool numbers and tool offsets. still grinding.
I would think all the tools relate or zero to a master tool. Code looks ok with just simple settings for tool numbers and operations. Im setting my templates up for a front tool post mounted tool.
Turret mount tool and paths would be flipped from picture below. and gang would be at 90 deg. Some operations have an approach option that has to be set right depending on how tool is located.
If this generates good usable code then im going to like this after I get some templates built out to import parts into.
Attachment 454666
Hi MD,
SC12 has been working pretty well for me in the lathe, though I mostly using it for new projects in my 1100/S3 these days. The last couple of lathe projects were simple threading ops and I just did those with the PP wizards.
I set up lathe tools for turret and a small gang setup and set the tool offsets for each by machining the OD and setting the X offset for that tool in the Offsets by measuring the OD and then entering the measured value in the box and pressing the "Touch" button on the screen. It's important to not change the X position for a tool until you've measured and entered that offset. I do all the tools for X in sequence and then do the Z offsets after that. I touch off each tool in Z against a a 0.001" piece of shim stock on a freshly faced piece of stock, enter the value (adjusted for the shim stock thickness) in the box on the offsets tab, enter "0.0000" in the box for Z offset and press or click the "Touch Z" button. I use the same faced surface to set Z for all tools. For a parting or slotting tool, I usually use a magnifier to line up the RH side of the insert or blade with the face. I suppose that you could also touch off on the LH side and enter the positive value of the insert or blade width as a zero off set for Z.
I use the gang tool holders for my drilling ops and use a Haimer in a 3/4" 5C collet in the spindle to center the spindle with the middle of the gang tool holder bore to establish X0. The advantage of that approach is that the X0 for a specific gang tool holder never changes for different size drills since they are all centered with respect to the gang tool holder bore.
I bought a Tschorn lathe tool setter some time ago and use that sometimes. My headstock seems to be mounted slightly off-axis compared to the bed and I have around 0.002" error in X in about 6" of Z travel. I keep meaning to fix that, or at least investigate more thoroughly, but all of my parts have been short enough with loose enough tolerances that it hasn't been a problem so far. The Tschorn is a much faster way to offset all of the tools for X and Z but it's a $600-700 tool. I happened across a deal on a like-new used one and snapped it up.
I'm fading fast here, so sorry if the above is just confusing gibberish. Ask, if you have questions and I'll try to provide a good answer.
Mike
Hi Mike
I dont think there is much a difference in SC lathe versions overall and the lathe post is old. They did rebuild the tools library. For the most part the documentation for the lathe operation setups has changed very little in years. It does seam to work good. Pretty easy to setup templates with same few tools for same few operations. Then import part and select surfaces for job assignment. Drag around tool lead in and outs as desired. Compile code and go make it. From what I see I should get up to speed in no time. Post generated code file had an extension of txt. This had me confused for a while but I let SC do its thing.
Thanks for the detailed information on tool setup and touch off!
I will need to step thru the process a couple times to get a rehearsed work flow. Will be using a front mount tool post holder. I mostly need to remember that all x values are negative and dro displays diameter value. Then pretty much follow your setup work flow only just one tool at a time. I like the idea of using Hamier for setting bore center on the drill/bore tool post holders. "wont need shims" screw adjust should be a bit simpler anyway.
Again thanks for the derailed response. Nice to get some first hand experience on how they setup their tools and machine.
I have a list of questions but will hold off until I see first hand how the machine works and behaves under different modes and conditions.
MD - just keep in mind that I could be doing things wrong, so take whatever I say with a grain of salt. I generally plod along with SC until I get the job done and learned to stop wasting time on trying to figure out why it doesn't work the way that *I* think it should.Quote:
Originally Posted by mountaindew
The main problem for me is that we lose power here often enough (or I clumsily bump the E-stop button), so that the lathe.resets and I lose my tool references. That means re-referencing everything and re-establishing offsets for at least one tool, possibly more if I have changed or need to change tooling. My 1100/S3 is accurate enough on the referencing for all 3 axes that I could just do that and run my program. My lathe repeats to (at worst) +/-0.015" in X and +/-0.045" in Z, resulting in needing to re-establish at least one tool offset at each reset.
I understand when it comes to Sprutcam. Most the time I can figure it out and get good results. I have spent many hours learning just 4th axis stuff and still struggle with the real complex stuff like flank milling. Just takes time to learn different parts of that program. Lathe section seams to be less work to setup parts then mill or router. For simple x-z axis machine anyway. And that is the reason for the most part just 2 axis to program not x,y,z,a . I have it simulating front tool post with tools in a visible sbl15 machine model. As for good code to make something. I have the mill and router cam setups refined enough that it comes down to how many clicks does it take to select the jobs and compile and save the files. Hope to do the same with lathe. It is the very reason I paid to stay current with the software.Quote:
Originally Posted by MichaelHenry
This is what I expected for tool offsets and machine setup at first anyway. Mill and router both home pretty accurate but I still set the offsets before running programs. I figured I would always need to set a master tool x-z offset when starting the machine up just like hamier probe on mill sets x,y,z,a and and everything works off that . Need to get a little time to develop some setup work flows. Figure out what works and what kind of strategy is best to get decent precision.
I also need to get all the tooling insert numbers And get the last part figured out and setup "lathe tooling". If its not described accurately, your not going to get the shapes and forms that go with the programed tool paths. Then get both sprutcam and PP working with same information. Should keep me busy for a while.
Quick question for mike or other readers.
The post looks like it uses g96 command in a way that would make machine start with a slow surface speed because the tool is changed at max x travel. Then as tool rapids into lead in position the spindle would want to spin up to match the rapid move!
Is this how pp conversational works?
Or Is this how other machines and posts work?
if so would this not put un needed stress on spindle motor trying to change and keep up?
Looks like machine should stay in rpm mode g97 until rapid move is over and it starts normal tool lead in. then switch to g96 and continue.
Is this correct or am I missing something?
Any help would be great
MD - sorry, never paid any attention to the use of g96, but AIR, the spindle does start at a slow spindle speed until X moves in for the cut. I'll try to make a note of the exact behavior the next time I run the lathe. If you are desperate for an answer, I can dry run one of my SC-coded.programs and a wizard-coded program.
Pay special attention to threading offsets. My threads are always far enough off to be useless without a lot of tweaking. Something to do with the typical insert threading tools coming to a sharp point and the code expecting a flat at that location but I haven't worked out the details yet. I've only used the conversational wizrds for threading so SprutCAM could act differently. I'm using Tormach (insert) threading tools, too, so it's annoying that the wizards and their defaults for a specific thread are so far off. It would be really nice, too, if we could edit the included thread formats for unusual thread forms, like the 2-1/8-6 male thread that I have to do this week.Quote:
Originally Posted by mountaindew
Version 14 has some threading changes, I might need to add a couple more chapters to my sprutcam notebook, just for tooling and tweaks.Quote:
Originally Posted by MichaelHenry
I went back thru the lathe sections in cnc programing handbook and sandvik training to help setup better operations. Also get up to speed and understand all the lathe codes and what behaviors they set. Things like multiple offsets for tools and other details are not covered or explained well in pp g-code manual,
One version 14 update released a month ago. From what i read it can turn threads in any form. I think it takes an accurate model of what you want. Then a tool that can make the profile in x number of passes. I have not been brave enough to install yet.
g96 question.
Mostly wondering how ,what and why the machine works with different codes that the sprutcam post puts in the programs. Then compare the file codes and format to cnc programing handbook by Peter Smid. Make notes and start looking in cam for setting that I might be missing then research and test.
The reason I asked about PP code it posts and if it used these codes. I don't have my 8l lathe setup yet and don't have pp hub installed so no access to lathe code yet. Not a big deal asking questions and researching at this point.
Nice to have someone with years of experience with both the lathe and sprutcam to get ideas from.
Thanks for the help and insight!
Mike or any sbl15 sprutcam users .
Setting up rigid tapping on 8l lathe and wanted to know if there is any settings to watch?
Long hand code or can cycles?
Seams to easy and I don't want to break tools
Thanks for any insight
I don't rigid tap in the 15L much, if at all, so no tips for you there. I have found that "long hand" works much better for me than canned cycles on the mill, so much so that I use that exclusively now. Can't remember why, though.Quote:
Originally Posted by mountaindew
Thanks for info Mike.
It was no problem, I just have to be careful and check spindle direction. Sprutcam wants to default the wrong direction.
Long hand is the only way I tried it. I also avoid can cycles because I was advised to long ago.
For any sprutcam tormach lathe users. I modified the tormach lathe post so it generates a program header with date, time, name and complete tool list exactly like the tormach mill and router post. If you want a copy let me know. I also sent tormach copy in case they want to use it. Or I can post instructions detailing mods if you want to edit your lathe post.
Hi MD,
I'm still using SC12 (though I have a legal copy of SC14) and just checked a recent TAP file generated with that. It lists all the info you mentioned at the start of the code/ Did SC14 revert to omitting that info? If so, I'll probably hit you up for the post or instructions once some current work is done and I get around to updating to SC14.
Mike
Hi Mike,Quote:
Originally Posted by MichaelHenry
The sl15 post that I have is the same one that has been distributed for years to me anyway. The lathe post from tormach I have creates txt files not taps. When you compile g code it shows no tool list or other info at start of a program file. I have used the mill and router posts for years and relied on looking at a tool list, date, time, and name information before i run program.
I just added the same exact header as the mill and router post generate. And i changed post so it generates files with tap extension not txt extension. Again to be more like mill but both extensions are valid.
Does your lathe post generate files with txt as file name extension?
HI MD,
No, mine has always generated *.TAP files. Maybe I am using an outdated post. Both my Tormach mill and SBL-15 lathe posts are dated 9/28/2019 which does seem a little dated. This is the header from a recent job for the leader:
%
(End Plate - Rev 2)
(POSTPROCESSOR: tormachPP)
(GENERATED BY SprutCAM)
(DATE: 4/7/2021)
(TIME: 7:09:16 PM)
(T# 31) (Dia 0.25) (1/4 Carbide 6-Fl EM) (Roughing waterline)
(T# 31) (Dia 0.25) (1/4 Carbide 5-Fl EM) (2D contouring)
(T# 100) (Dia 0.25) (1/4-in Carbide Spot Drill) (Spot Drill)
(T# 125) (Dia 0.281) (1/4-20 Body Drill) (1/4-20 Clearance Drill)
(T# 31) (Dia 0.25) (1/4 Carbide 6-Fl EM) (Rough NPT Clearance)
(T# 31) (Dia 0.25) (1/4 Carbide 6-Fl EM) (Finish NPT Clearance)
I get same on mill but lathe post was generating only this
%
O0001
(billetSteppedindicatormountv1)
N10 G18 G40 G80
(Lathe facing)
N20 G20
N30 G54
N40 G30
N50 T0808 (SCKCR08-2A)
N60 G96 D1413 S185 M03
N70 G00 X6. Z3.
N80 X1.2042 Z0.1121
N90 Z0.
.................................................. ........................................
now it generates
%
(POSTPROCESSOR: Tormach L15 Slant-PRO_RevC1)
(GENERATED BY SprutCAM)
(DATE: 4/29/2021)
(TIME: 5:04:49 PM)
(T# 8) (SCKCR08-2A) (Lathe facing)
(T# 1) (SDJCR08-3A) (OD Roughing)
O0001
(billetSteppedindicatormountv1)
N10 G18 G40 G80
(Lathe facing)
N20 G20
N30 G54
N40 G30
N50 T0808 (SCKCR08-2A)
N60 G96 D1413 S185 M03
N70 G00 X6. Z3.
N80 X1.2042 Z0.1121
N90 Z0.
.................................................. ..........
I dont know what the difference is my tormach l15 post has date of 21.03.25
but from what i have seen the date is all that has changed in a few years.
I looked at code i did a couple years ago and it is same as my first post no header. and in txt format
Weird, I wonder why Sprut or Tormach dropped support for header info from just the lathe? I'm guessing that Tormach never got back to you on your message about the issue.
BTW, Tormach has a Discord "forum" for SprutCAM support. Not much traffic there, though I seem to have lost access to the Support channel there.
https://discord.com/channels/6649535...53559544102953