First Horizontal Program

[Radical1]

Hi all, I have a program to do for a Kitamura horizontal...my first horizontal program, I usually do verticals. having trouble figuring out the procedure. I have one part to do in three positions on each face of a tombstone (total of 12 parts). I originally programmed one part in top WCS and top plane in the correct position relative to a lineup hole on one face of the tombstone. I am having trouble getting the  the program to post the code to rotate the toolpath to the other faces. the first rotation is starting at B-90.0. I am just using the standard M\C 4 axis horizontal post.

 

I hope this is enough info and that I am just missing one or two steps, any help would be greatly appreciated.

 

Richard

[Colin Gilchrist]

For a "standard" horizontal post, you need to program with Top WCS, and FRONT Tool/Construction Plane. This would show your tool coming in from the Front for B0. Then you can program using Right for B90., Back for B180., and Left for  B270., and the post will calculate the correct B output for you.

[Radical1]

I kind of thought that, so that means I have to translate the geometry to all locations and retoolpath (new word) at each new position, I was hoping to use the transform toolpath to do this, but it sounds like I can't.

 

How do I account for the lineup hole in the first face? Would this be the MasterCAM origin or would the center of the table be the origin? I know the location of the hole relative to machine home.

[Colin Gilchrist]

It really depends on your individual parts. How are they mounted (vise or dedicated/modular fixturing)? Are you worried about clearances from one station to the next? And are you only doing positional work (3 + 1), where you rotate the B-Axis to a fixed position, then clamp, or do you need to do Simultaneous linear and rotary motion?

 

Typically, you would program the part with just a Toolplane, and Work Offset. The work offset is local to the part, so when you mount the part on the fixture, you would probe or set the location with a dial indicator. The coordinates of the NC code are relative to the Work Offset location, so as long as you dial in the part correctly on the machine, you don't have to worry about programming from the center of rotation.

 

When I program a horizontal machine, I make sure I model my tombstone, and I program from the center of rotation. This does require that you physically measure your tooling on the machine, so that you can model it accurately. As long as you draw everything in Mastercam to match the "real world", you then have the advantage of only needing to program using a single Work Offset, and all the coordinate locations come from the center of the tombstone. It takes more work to setup your program this way, but you get some good benefits by taking the extra time. One of the biggest reasons I program this way for a horizontal is to take advantage of using "G10" lines to set my work offsets "automagically" in the header of my program. It saves the operator from having to enter work offset locations manually, but might not be worth the effort to setup if you aren't running repeat production jobs.

 

Hope that helps,

 

Colin

[Radical1]

Thanks Colin, you have been a great help! I did as you suggeted with the toolplanes and WCS and it does as I wish it to. I even tried to use the toolpath transform and it will work nicely as well. All I have to do is rechain all the toolpaths for the proper planes.

 

Thanks again

Richard

[crazy^millman]

Thanks Colin, you have been a great help! I did as you suggeted with the toolplanes and WCS and it does as I wish it to. I even tried to use the toolpath transform and it will work nicely as well. All I have to do is rechain all the toolpaths for the proper planes.

 

Thanks again

Richard

No you can re pick the Plane for the already programmed operations. If incremental on everything then regenerate and done, if absolute check all things in the linking parameters for the toolpath.

 

We also program machines for customers this way. We then leave up to them to decide if they want to make it harder on themselves or not. We gave our customers the best process we think and go from there. Why add extra work to programming a part with many different offsets and such? One work offset is really a good practice to be in.

[Radical1]

Thanks for that Ron, I am going to play with the programming a bit. It sure would save a lot of work, just got to get used to thinking four machining planes.

 

Richard

[Sticky]

Why add extra work to programming a part with many different offsets and such?

 

There are more reasons to use multiple offsets then there are to use just COR. The only reason to use one offset is laziness, but it will work fine for many things. In process inspection, tool blending, tight tolerance work, castings, weldments etc do not lend themselves to programming off COR only.

[Newbeeee™]

There are more reasons to use multiple offsets then there are to use just COR. The only reason to use one offset is laziness, but it will work fine for many things. In process inspection, tool blending, tight tolerance work, castings, weldments etc do not lend themselves to programming off COR only.

Previous place we had 4x hitachi horis and jobs would go from machine to machine (because of bottlenecking).

We found the trouble with COR was that the machines wouldn't rotate perfect about the centreline (they'd had a few 'bumps' along the way...), so we changed practice so we had an individual datum per index (predominantly B0, 90, 180, 270). 

FWIW, we don't have horis at the place I'm at now, but we prog with a separate G5# per index for all our vertical/4th axis work. This also helps for when a fixture doesn't run spot on when it goes back up for the next time.

[Sticky]

^ Absolutely. All machines move, not just thermal axis growth, but spindle and squareness as well.

 

Using offsets makes life for the operators and setup personal much better as well, from proving programs out to fixing parts or fixtures.

[crazy^millman]

There are more reasons to use multiple offsets then there are to use just COR. The only reason to use one offset is laziness, but it will work fine for many things. In process inspection, tool blending, tight tolerance work, castings, weldments etc do not lend themselves to programming off COR only.

 

The only reason is laziness? Really?

 

Okay glad I have learned something I never knew.

 

I am sure some of the 28 index parts we program will benefit greatly from the operator having to pick up the 28 different fixture offsets.

 

When center of rotation is correctly picked up and accounted for then you should be able to repeat your process day in and day out with no problem.

 

I also never said COR was the only way. I said it is a good practice to be in. That does not make it the only way it makes it a good way.

 

Have a great day.

[Newbeeee™]

Ron,

To elaborate on the horis at my old place.

We couldn't afford to get a tech in to fix them because the place was constantly insolvent. We had to get by and get the job done.

The place went pop 3 times starting again the following day until it finally disappeared.

[Sticky]

The only reason is laziness? Really?

 

Okay glad I have learned something I never knew.

 

I am sure some of the 28 index parts we program will benefit greatly from the operator having to pick up the 28 different fixture offsets.

 

When center of rotation is correctly picked up and accounted for then you should be able to repeat your process day in and day out with no problem.

 

I also never said COR was the only way. I said it is a good practice to be in. That does not make it the only way it makes it a good way.

 

Have a great day.

 

 

Yes the only reason is laziness, there is no advantage using COR only except in programming setup time. It does take a bit longer when programming to setup multiple offsets, but that is the only disadvantage.

 

If the operator is going out and picking up all the offsets you are doing it wrong. All the offsets should be in the header of the program using G10. This gets populated by the different planes or wcs' in the view manager.

 

As for day in day out, it depends on the type of parts, plus or minus .002" or more, on a good machine sure, tighter then that, especially lights out, no.

[Sticky]

Ron,

To elaborate on the horis at my old place.

We couldn't afford to get a tech in to fix them because the place was constantly insolvent. We had to get by and get the job done.

The place went pop 3 times starting again the following day until it finally disappeared.

 

 

Wouldn't matter anyways. Trying to get 3x machines truly square within .0002" or less, and getting the grid shifts set so that you can run identical offsets on each machine is a fools errand. If one machine looses .0002" square in YZ you could be making parts with surface more then .001" undersize (or worse) if the datum is tied to a feature on the side of the part.

[Mick]

I programmed a Toyoda FMS with two 1050S's for several years. We manufactured several parts on one fixture, and on those several parts some had to have several local work offsets to provide blending for the castings.

 

COR wouldn't have worked. In fact, several parts in the past had been programmed with COR and they ended up being more troublesome for the operators to set, so we changed those to local work offsets.

 

Ron, it is my interpretation from your post above that says "a really good practice to be in" that conveys that COR is the recommended method of horizontal programming. However, imho, it isn't. It just isn't as flexible, especially with multiple parts.

[crazy^millman]

Yes the only reason is laziness, there is no advantage using COR only except in programming setup time. It does take a bit longer when programming to setup multiple offsets, but that is the only disadvantage.

 

If the operator is going out and picking up all the offsets you are doing it wrong. All the offsets should be in the header of the program using G10. This gets populated by the different planes or wcs' in the view manager.

 

As for day in day out, it depends on the type of parts, plus or minus .002" or more, on a good machine sure, tighter then that, especially lights out, no.

 

Okay well I be sure and go tell all the companies doing it they are wrong. Well glad to know I am not making it harder on myself doing it the non lazy way.

 

I am not the one going out and picking up anything. I am giving the customer what they demand. I have personalty programmed parts off the center line of rotation for a long time. I do it for Mill/Turns, 5 Axis Trunnions, VMC with a 4th Axis and HMC with a 4th Axis. Every time I have done it I have been able to hit tolerance and size with no issue and yes lights out as well.

 

Yes it all falls under the same umbrella.

 

I was talking to someone about this topic. I like what he had to say. "You want to find the most efficient way to do something give it to the laziest person" :cheers:

Edited July 20, 2015 by 5th Axis Consulting

[crazy^millman]

I programmed a Toyoda FMS with two 1050S's for several years. We manufactured several parts on one fixture, and on those several parts some had to have several local work offsets to provide blending for the castings.

 

COR wouldn't have worked. In fact, several parts in the past had been programmed with COR and they ended up being more troublesome for the operators to set, so we changed those to local work offsets.

 

Ron, it is my interpretation from your post above that says "a really good practice to be in" that conveys that COR is the recommended method of horizontal programming. However, imho, it isn't. It just isn't as flexible, especially with multiple parts.

 

Okay take what you want from what I am saying.

 

I offered advice to help someone get moving on a job. I still stand behind it is a really good practice to be in. I have not said it is the only way.

[Newbeeee™]

So to go a little OT as we're debating this here, for mill-turn work, would it be standard practice to prog from C/L?

I'd assume it would be less problematical than a hori, as the lathe spindle would obviously be on centreline, and I'm assuming bar/billet work here and not a fixture set in the chuck (which could run out)?

Just curious.

[BenK]

I just have one question. Would you program a 5 axis machine with multiple offsets as well?

[crazy^millman]

 

So to go a little OT as we're debating this here, for mill-turn work, would it be standard practice to prog from C/L?

I'd assume it would be less problematical than a hori, as the lathe spindle would obviously be on centreline, and I'm assuming bar/billet work here and not a fixture set in the chuck (which could run out)?

Just curious.

 

 

It is the same thing. If you know where center line of your 4th Axis is then it is no different. You come up with a standard way to program everything you do. Once you understand where C/L is on any machine you then understand how to design, machine and work that way. Now you carry a common process across many different ways to machine and manufacture parts. Not one way here and other way there and maybe this this way over here. Carries across many different controls and also allows for WSEC, CYCLE800, G54.4, G43.4, M200 or other methods that take the one workoffset mind set to the machine tool and allow you to adjust for error like mentioned when it comes up.

 

But again it is the lazy way to go about doing work so it must be a stupid way.

[Newbeeee™]

I just have one question. Would you program a 5 axis machine with multiple offsets as well?

My mate does on his MAM72 to lesson chasing tolerances from face to face.

[crazy^millman]

My mate does on his MAM72 to lesson chasing tolerances from face to face.

 

See that is different. Is the programming done from the same COR or is it done with G54 being one place and G55 being a different place? COR means all programming done for all the different places uses the same common point for programming. Calling out different workoffsets or G10 for them is the same amount of work. You still need to make planes for rotations and you still need to define things the difference is you can either work from one workoffset doing it that way or not. Once you understand how it works and then define your process around it to support it then makes everyone's life easier. Doing a plate with 4 holes and no indexing then no I would program it like a 3axis which yes I do treat different. Doing a manifold with 28 cross sections and 14 different ports then I would program it from one point. That one point would be the COR.

[Sticky]

You said:

 

 

 

I am sure some of the 28 index parts we program will benefit greatly from the operator having to pick up the 28 different fixture offsets.

 

 

Now you say:

 

Okay well I be sure and go tell all the companies doing it they are wrong. Well glad to know I am not making it harder on myself doing it the non lazy way.

 

I am not the one going out and picking up anything. I am giving the customer what they demand. I have personalty programmed parts off the center line of rotation for a long time. I do it for Mill/Turns, 5 Axis Trunnions, VMC with a 4th Axis and HMC with a 4th Axis. Every time I have done it I have been able to hit tolerance and size with no issue and yes lights out as well.

 

Yes it all falls under the same umbrella.

 

I was talking to someone about this topic. I like what he had to say. "You want to find the most efficient way to do something give it to the laziest person" :cheers:

 

You make it sound like you don't know how it works. Maybe you do, but when you contradict yourself by 180* it makes it hard to follow what you are saying.

 

 

 

So to go a little OT as we're debating this here, for mill-turn work, would it be standard practice to prog from C/L?

I'd assume it would be less problematical than a hori, as the lathe spindle would obviously be on centreline, and I'm assuming bar/billet work here and not a fixture set in the chuck (which could run out)?

Just curious.

 

 

C/L or COR is where you start, just like on a mill. If I can get away with just using COR on a mill turn I will, if it's a tight tolerance production job I'll use multiple offsets right from the start. COR moves on a lathe just like it does on a mill, which is why it is particularly poor practice when working on parts that have opposing faces, or a datum on one face with other faces tied to that datum.

 

 

I just have one question. Would you program a 5 axis machine with multiple offsets as well?

 

Yes it is what I do. I don't do much in the way of surfacing, but if I did I would use COR for the surfacing tool paths and then a local offset to inspect the surface afterwards.

[BenK]

Sounds to me like you have an issue finding center of rotation. 

 

I program off center and I still need to construct all the same planes. Only difference is I don't set a different offset for each index. Its the same amount of work for the programmer. Difference is you need to make sure all your fixtures are built correctly. Your process is only as good as the work you put into it up front.

[crazy^millman]

Sticky man you really need to learn how to read. You keep generalizing my comments to mean what you want them to mean and not what they are saying.

 

I have a part right now with 11k surfaces on it. It has about 400 different pockets at different angles on it. If I program it correctly and do my job correctly it like the 100's of others parts the customer has run using one workoffset will come out correctly. Following your mind set it would be 400 different G10 lines for each one. Following my mind set it will be one.

 

You have no clue about my experience or my abilities and not sure why you think attacking or calling it into question is important. You are more than welcome to walk a few weeks in my shoes and get a good idea what I do and do not know. Those who know what and where we are working have confidence in our ability to get the job done.