I've been an occasional poster here for about seven years. I'm not a "regular" but a few of you may recognize me. This is my first question in a while.
Please forgive my ignorance, I've always worked with mills, I've never really paid any attention to lathes.
I'm accustomed to manual center lathes. Generally the spindle turns toward you, the tool is on the operator side, cutting edge up etc. I've used them plenty.
I do plenty of production and prototype CNC mill programming and setup.
I'm lost on a CNC lathe.
We have a small slant bed CNC gang lathe I need to figure out how to operate. It is for low volume parts (200-2000 lots) so we can bring "in house" certain components that we need better control of delivery times.
My question is this. Do you typically run the spindle toward you with a cutter in front, or away from you with a cutter behind or toward you with a cutter upside down and behind?
I'm not asking for a long dissertation that would take you forever to type out, but if you could spare 20 seconds to give somebody starting at zero (on lathes) a few pointers I would be very appreciative.
Polymer Man wrote in news:4b4b633b-b987-43f8-9042- snipped-for-privacy@m3g2000hsc.googlegroups.com:
I always run the tools face up, so that the forces are going into the bed and not trying to lift the slide off the bed. Some do it differently. If the slide is at the rear as you stand in front, the machining happens on the backside of the spindle, and the spindle turns clockwise, looking from the tailstock.
Upside down and behind with the spindle turning towards you. One advantage, the spindle doesn't have to stop and reverse to do drilling. Another, the chips are headed in the right direction (down) After a couple of days, this will seem normal to you. A couple of other points: a common mistake is to have tools hanging out too far and contacting parts of the machine. Cut long boring bars to the size needed for the job and use stub drills whenever possible. And never have stock hanging out of the end. Even a 1" bar will bend at high revs.
Polymer Man wrote in news:4b4b633b-b987-43f8- snipped-for-privacy@m3g2000hsc.googlegroups.com:
On a small gang tool lathe it doesn't really matter which side of the part you turn from.
There is something of an art to laying out the tooling on a gang tool lathe. If you are working from bar and parting off, then usually your cut-off tool needs to be at the end of the table (bottom end in your case).
Usually you try to lay out the tooling in such a way that chip to chip times are minimized. You have to be mindful of the clearances. And you want to work progressively from one end of the table to the other.
You also want to economize on space as much as possible when laying out the tooling. There are some tools made specifically for gang tool lathes that perforn multiple functions. Such as boring/turning bars. Twin insert bars that can turn from either side. There are also combination drilling/boring/turning tools.
In general you want to start at the far end of the table and lay out the tools in the following sequence:
1) Bar feed
2) Rough face and rough turn
3) ID work - Spot drill, drill, ream, bore, tap, etc.
4) Finish face and turn
5) OD threading
6) Re-trace thread chfrs.
7) re-cut finish thread pass
8) Any other OD ops. Grooving, knurling, etc.
9) rough any features behind shoulders
10) Finish features behind shoulders
11) Cut off
Of course the work will dictate the best lay out but this is a decent "rule of thumb" starting point.
In the above lay out I would rough turn from the front side of the spindle. If you use a twin bar, you could then use the other side to finish turn from behind which would leave the threading tool in position to single point the thread from the front. Then re-cutting the thread chfrs the finish tool is still right there, then you jump back to the threader and take a final finish pass.
Then you could move to a groove tool used from the back, then to another groover or knurl used from the front, and so on. This way you minimize the chip to chip time and economize on table space.
The main thing is to use all right hand tooling and run the spindle in the CW direction only. Since you are using a slant bed gang tool, I would mount right hand boring bars face down so that the cutting edge will be at the high side of the spindle rather than the low point. This will help with chip clearance.
Keep your tool overhangs as stubby as possible and set all the OD tools to as near the same Z-plane as possible. Unless you gain some advantage by staggering them. It's best to start with a pencil and paper and plan out the sequence of operations while considering the table lay out, tools available, and efficiency.
I can't think of any other advice off the top of my head but if you have a specific question fire away.
Thank you all for the excellent input, I appreciate it.
Dan, it took me a few readings to absorb all that, but I feel like I have a much better handle on this now. Thank you.
If anybody else has any input, thoughts, .02, etc, I'm all ears, but I have a pretty good starting point now.
A minor question if you want to entertain it:
On a gang lathe, when shifting to different tools, is that normally done with a different work offset? Is that called with G54, G55 etc? It will probably be obvious once I start fishing around in the control (Meldas M50).
Are you planning on running bar feed or chucker type work or a combination of both?
Complete parts or second op?
One family of parts, a couple families or wide variety mix?
Job quantities, styles & how often do jobs repeat?
In your situation and mix of work, can tool positions be standardized without adversely effecting (tool to tool) cycle times?
If you are running family of parts then your set up will be simple since you will be able to use the same tool positions and maybe only need to change a drill, threading tool adjust bar puller for each job.
If you are running a couple different families then you can make quick change sub plates with locating pins where the tools are set for each family (may be a viable option for you depending). Offsets can be uploaded and downloaded with the program.
Each tool has it's own offset, X measured to spindle centerline and Z to a set reference point or some use the front or back of the part.
There will be a "work shift" not sure on your machine if it's G54 but it will work the same shift in Z, X is usually 0.0. How it is utilized is dependant upon how you decide to set your tools.
Similar to a mill once tools are measured and set you don't need to set them again you just input the "work shift" Z amount when you change to new job.
Make sure in your CAM system (write) to make a post that will square off rapids so you don't erase (break) a line of tools. As stated before by others you would like to have all tool lengths at the same distance however that is not always possible.
Depending upon your situation you may have a Drill hanging out 4", OD tool 1-1/2" bore bar 2-1/2" and cutoff tool 3" you need to insure you don't rapid into them when clearing the part and changing tools.
There are variations depending but as a general rule rapid towards the part I would want to (square off) rapid x first then Z towards the part. After tool is finished safely clear X then rapid to tool change position Z (safe Z) call up next tool rapid X then Z towards the part.
You should enjoy learning a gang tool lathe, it is a nice change, a challenge and you will be learning something new.
Set X & Z zero from machine Zero, calculate tool offsets sets from there. (Same as using G50 in the old days)
There will be (should be) a tool offset measure function in the controller.
At machine startup Operator only needs to Home machine, zero out counter. To measure tools: Start spindle (if necessary) Call up tool (for this example T#1) Touch off or face part On tool measure screen highlight T#1 Input "measure Z.0" (If there is .003" of material to come off the face then input "measure Z.003")
Exception #1: If using G30, at start up you need to move the slide to G30 then zero out counter.
Exception #2: if you are using a reference point for Z touch off the reference point not the edge of part.
Setting X offsets are nearly the same except the need to indicate X.0 for drill/tap centerlines.
If using quick change sub-plate & or tooling specific to a job uploading and downloading offsets are definitely the way to go.
Here is an example of a simple Gang Tool multiple Tool holder that looks to be job specific as an example.
formatting link
This is the first photo I could find, not the best way to go IMO (just using it as a visual). I would want dead stop or locating pins/holes so the change over is quick and uploaded (saved) offsets accurate.
What I meant by standardized is something like this:
Tool positions can always, almost always, stay in the same position something like this;
T#1 drill T#2 spot drill T#3 bore bar T#4 open (tap, id thd, ID, OD groove etc) T#5 OD turn T#6 OD thread T#7 Cut off T#8 bar puller/bar stop
If you can determine NOW standard positions for most tools you will use, based upon your mix of work it will make your life much easier.
I use G10 more on mills than lathes, very powerful tool, particularly when running multiple parts. I have programmed and used it for running up to 100 parts at a time on VMC using pallets. Unload, Load one pallet of 100 parts while the other pallet is running.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.