High accuracy drilling / boring

[Mike Whitten CAD/CAM Contractors]

Hello,

 

Contrary to my beliefs, my Surfcam friend over here believes that it is more accuarate to move to a position for "High accuracy drilling / boring" in feedrate rather than rapid. Maybe he is correct? He is used to Surfcam which has a type of drilling routine that basically does a virtual "G60" uni-directional approach at feedrate. It will start at .10 away from the hole and move up to it in feedrate and then drill the hole.

 

I am wondering if there is way to do this in Mastercam? He is trying to do this in Mastercam right now.

 

I am playing with it and have found ways to do it using "Point" but we want to know how to do multiple holes quickly.

 

Any help is greatly appreciated.

 

Thanks,

 

Mike

[mayday]

I have yet to see the need for it on a good quality machine. only wore out ballnuts/leadscrews with backlash will cause this.

[Trevor Bailey]

On most machines, there is a "true positioning" code. The machine will rapid to specified location and automatically take "lag" out by itself. May want to check the books for your machine and don't waste your time with modifiing code.

[chris m]

Not trying to be a wisea$$; but why not just USE G60?

 

Additionally, most CNC machine tools default to Exact Stop in rapid moves where they do NOT in feed moves so I'd say that you friend may not be completely on target there.

 

We currently use G60 in our Okumas and ream holes within a tolerance of .0008 true position to an existing feature all day long

 

C

[Mike Whitten CAD/CAM Contractors]

I agree with everyone so far as this was what I was telling him but...

 

Thanks,

 

Mike

[Mike Whitten CAD/CAM Contractors]

I have an urgent issue at home, I will be back later.

 

THanks,

 

Mike

[Keith Graydon]

We use this method on our SIP manuel Jig borer.

All ways unidirectional positioning

Finefeed the last .100 or so.

a CNC machine with an open loop system may benefit from this technique but i doubt a machine with a closed loop system (scales) would.

 

How close do you need to be?

[Tim Johnson]

If you're using an encoder or a resolver to find position then your friend might be right. If you're using scales it should'nt matter.

[Guest CNC Apps Guy 1]

You'd need to do some post tweeking to get the G60 in there. It's entirely possible though. How the G60 works is it over shoots the hole by a certain distance (usually 1mm), then moves back, effectively removing any backlash.

 

In all honesty though, if the machine is in good condition, you spot drill the hole, your drill has >.0005 TIR you should be able to hold true position of .001" or better.

 

Tell Surfcam boy to put the crack pipe down he's going to hurt himself and/or somebody else.

 

JM2C

[Mike Whitten CAD/CAM Contractors]

I am back. I was busy getting my house burglarized. I had to get to my house while the police were still there. The low lifes took my oxy set up and tried to cut the hinges off of my Browning Gun safe. I lost quite a bit of stuff but lucky they did not get the firearms. This is why my house is for sale. I am getting ready to head out to Northern Nevada, maybe Elko or something.

 

Mayday,

quote:

---

I have yet to see the need for it on a good quality machine. only wore out ballnuts/leadscrews with backlash will cause this.

---

My experiance has shown me that even on the perfect machine, there will generally be some backlash or reverse backlash( backlash comp may be wrong). SInce we are trying to hold true position or .0003 or so, everthing counts. What I normally do is to let the CMM teell me what is happening. At this point, if my machine repeats, I just lie to it. What it is.. is What it is.

 

 

Trev,

quote:

---

On most machines, there is a "true positioning" code. The machine will rapid to specified location and automatically take "lag" out by itself. May want to check the books for your machine and don't waste your time with modifiing code.

---

He is used to Surfcam doing it so this is what he wants.

 

 

chris m,

See above and also:

quote:

---

Additionally, most CNC machine tools default to Exact Stop in rapid moves where they do NOT in feed moves so I'd say that you friend may not be completely on target there.

---

This is exactly it! I told him this. I think the machine will repeat better in rapid?

 

Keith,

quote:

---

a CNC machine with an open loop system may benefit from this technique but i doubt a machine with a closed loop system (scales) would.

---

Thanks..we don't have scales.

quote:

---

How close do you need to be?

---

The customer is so freaked out that they say want it closer than any CMM can check it!

 

Tim,

quote:

---

If you're using an encoder or a resolver to find position then your friend might be right. If you're using scales it should'nt matter.

---

This what Keith was saying. You guys may be right. Thanks

 

James,

quote:

---

You'd need to do some post tweeking to get the G60 in there. It's entirely possible though. How the G60 works is it over shoots the hole by a certain distance (usually 1mm), then moves back, effectively removing any backlash.

---

Thanks but he wants Mastercam to have a cycle for this!

 

also

quote:

---

In all honesty though, if the machine is in good condition, you spot drill the hole, your drill has >.0005 TIR you should be able to hold true position of .001" or better.

---

We need it to be 5 times closer than that.

 

also

quote:

---

Tell Surfcam boy to put the crack pipe down he's going to hurt himself and/or somebody else.

---

I almost fell off my chair when I read this one! This is what we will call him from now on. He is a good guy, he is just a loyalist like we are. Everytime I try to show him the power of Mastercam, he just brings up features like this.

 

Thanks to all!

 

Mike

[Rekd™]

You did say true position of .0003, right?

 

No software in the world is going to get a standard mill to hold that kind of tolerance, sorry. You CAN get mastercam to do pretty much whatever you want, just put up a sample of code that surfcam is putting out and I'm sure we'll come up with several ways to do it with our software.

[Rekd™]

quote:

---

He is used to Surfcam doing it so this is what he wants.

---

Oh.

 

So this is what you're dealing with, eh?

[Mike Whitten CAD/CAM Contractors]

Rekd,

 

Yep! this is what I am dealing with. It will all come out OK in the end though as Surfcam is good but not good enough.

 

Anyhow, all the what he needs is to rapid the tool to X-.1, Y-.1 from the hole and feed over to the hole and drill it. I was able to do it perfectly using "point". I was just wondering if there was a was to sub it or something with a standard post so that I can just do it. This is not an urgent issue because there are many other ways to do it I just thought I would post and see if I may have missed something.

 

Thanks,

Mike

[Rekd™]

You could define a custom drill cycle to do it easily. Just offset the XY amount in the post, then as the drill cycle starts, it feeds to the hole from the same direction.

 

IMNSHO, it's your customer that needs to put down the crack pipe.. What material are you trying to do this with?

[Mike Whitten CAD/CAM Contractors]

Thanks Rekd,

 

A drill cycle would be nice but this is not what he wants. Thanks

 

The customer is physco, the part is desiged wrong!

 

The material is 304

 

thanks,

 

Mike

[Rekd™]

Mike, I'm lost. He wants to rapid past a hole, feed to position, do the canned cycle, and on to the next hole? Like..

 

G90G0X.1Y.1

G1X0Y0F3.

G81ZBLAH BLAH BLAH

G90G0X5.1Y5.1

G1X5.Y5.F3.

G83ZBLAH BLAH BLAH

 

??

 

Like I said, create a custom drill cycle, what's easier to do drilling operations than a drill cycle? You can create a custom drill cycle to do this or just about any other thing your machine is capable of doing.

 

:shrug:

[Scott Bond]

Hi Mike

This was a great question,,and guys these

are very good answers. I use the true postion

hand edited in once every 6 mounths when I

need it. I avoid the lie to the machine style

only because it forces the stored program to be false , and it won't run for poop next time.

 

I'm sure your customer isn't getting what he

thinks he's getting if no CMM could check what

he wants.

 

As for the Surfcam programmer,,,I'm sure that after we give a solution that produces the same (lame) style with the exact same code as the the Surfcam code, then he will say that the Surfcam parts are more accurate .

[iowajim62]

Mike,

Sorry to hear about your house.

 

quote:

---

SInce we are trying to hold true position of .0003 or so, everthing counts.

---

You are right everything counts especially considering most mills (vmc or hmc) have advertised repeatibility of .0002 per axis.

All good ideas offered up for your Surfcam buddy to check but I would say that tolerance will only be achieved on a jig grinder or jig borer.

Good Luck

[Mike Whitten CAD/CAM Contractors]

Rekd,

quote:

---

Mike, I'm lost. He wants to rapid past a hole, feed to position, do the canned cycle, and on to the next hole? Like..

 

G90G0X.1Y.1

G1X0Y0F3.

G81ZBLAH BLAH BLAH

G90G0X5.1Y5.1

G1X5.Y5.F3.

G83ZBLAH BLAH BLAH

---

This is exactly what he wants.

 

and

quote:

---

Like I said, create a custom drill cycle, what's easier to do drilling operations than a drill cycle? You can create a custom drill cycle to do this or just about any other thing your machine is capable of doing.

---

I will look at it but the whole thing was to be able to do it with a standard post. Our posts are just modified MPmaster posts and they work great but to change this would still take a while as I would have to change about 10 different posts.

 

Thanks for the good ideas Rekd.

 

Mike

[Mike Whitten CAD/CAM Contractors]

Scott,

 

 

quote:

---

I avoid the lie to the machine style

only because it forces the stored program to be false , and it won't run for poop next time.

---

I believe that a machine could probably do something different depending on the current conditions. If our CMM says it .0002 off and there CMM says it is .0002 off then it is .0002 off. So the program does not matter it is .0002 off. Therefore, lie to the machine.

 

Thanks

[Mike Whitten CAD/CAM Contractors]

Jim,

quote:

---

Mike,

Sorry to hear about your house.

---

Thanks, I am getting used to these things as I have had a very bad last three years.

 

and

quote:

---

You are right everything counts especially considering most mills (vmc or hmc) have advertised repeatibility of .0002 per axis.

All good ideas offered up for your Surfcam buddy to check but I would say that tolerance will only be achieved on a jig grinder or jig borer.

Good Luck

---

they used to make them on a jig grinder but we must make them on a mill.

 

Back in the old days, we used to build stuff to .0002 on old crappy shizuoka mills. the trick is that you must be able to check the part.

 

thanks,

 

Mike

[Teh Bear without Brains kinda idiot]

~~~~~~~~~~~~~

You'd need to do some post tweeking to get the G60 in there. It's entirely possible though. How the G60 works is it over shoots the hole by a certain distance (usually 1mm), then moves back, effectively removing any backlash.

 

In all honesty though, if the machine is in good condition, you spot drill the hole, your drill has >.0005 TIR you should be able to hold true position of .001" or better.

 

~~~~~~~~~~~~~~~`

+1000 to james

Also consider this :

Do not use g81 ,use a cycle with stop at the bottom ,m5,orientate the spindel ,move a bit in one axes to distance cutter from hole and remove it from hole ,if your machine can do it .

You eliminate a backlash and deviation of Z axes

and spindel (g83 or g81 will do it 2 times worse it will leave traces or if you will slow G0 will bore it wrong).

This is very important especially with machines with Z moving table .

That`s what I do

And you will get more accurate hole

All this thread stinks a bit ,this guy is a real

%%%%A$$ ,I feel sorry for you .

And the home robbery ....

I wish you good luck and a lot of patience ,and critical approach to all sort of advices from everyone ,including my humble person

 

HTH

WTHH

[chris m]

Sorry about the break-in Mike; that sucks

 

quote:

---

SInce we are trying to hold true position or .0003 or so, everthing counts

---

Yikes! That's a tall order, even with glass scales; without scales it'd be a real xxxx. Is that a true position to another feature that you're machining in the same operation, or is it to a pre-existing feature? Hopefully something else that you're machining at the same time; otherwise I think that you're porked.

 

We don't have scales in our Okumas and we do see TP numbers under .0004 on some of the parts we run [to a pre-existing feature that we probe and WOFS shift on each part] but some of them brush up against the .0008 tolerance (some of this is due to positioning error, some to cutting tool deflection and runout, some due to probing without scales]. If we were doing the 2 holes and the datum at the same time I have no doubt that the machine would be under .0004 TP all day using the G60 command. I think if it was me I'd write an mi into your post for unidirectional positioning so you could output G60 in the ops that you want it and forget all that longhand code crap.

 

If you are going to feed everywhere I'd look through the machine manual and see if the machine is defaulted to Exact Stop for feed moves or not [i'd say not]. If it isn't, put the G64 [or whatever the Exact Stop command is] in before you do this or I think your feed-up approach will actually be LESS accurate than rapid.

 

C

 

BTW, it you're boring and not reaming the holes I'd definitely say that Fine Boring is a must as the bear mentioned above

[McRae]

If the part has a 0.0003 TP Tolerance - Jig Bore it - These machines are made for this type of work. If the customer truly needs that tolerance, they should be willing to pay for it.

 

If you want to be statistically accurate to with the 0.0003 then you would have to have a repeatable result well under the 0.0003 and my stomach would be in knots if I had to run it on some of our machines. Here is the other thing, has the customer demanded an MSA off of the CMM? How do you know the checking device is capable of this type of a measurement?

[Mike Whitten CAD/CAM Contractors]

WTP,

Thanks for all of the good advice. Everything helps when you are trying to hold tenths.

 

 

chris m,

quote:

---

Is that a true position to another feature that you're machining in the same operation, or is it to a pre-existing feature? Hopefully something else that you're machining at the same time; otherwise I think that you're porked.

---

It is just two holes. Thanks for all of the info.

 

 

McRae,

quote:

---

If the part has a 0.0003 TP Tolerance - Jig Bore it - These machines are made for this type of work. If the customer truly needs that tolerance, they should be willing to pay for it.

---

This is what they used to do. Here is the thing I am not understanding about the Jig bore. How do you know if the part is correct? I don't trust anyone! So..you still have to check it. If you have to check it than you may as well do it on a mill. I have never had a part that we could not hold tolerance. I am not saying that there is not one, just that it has not happened to me yet. The part he is trying to make is a very simple part. If you have a setup to check the part then you can get a pattern on the machine and then just lie. It has always worked for me so far.

 

and,

quote:

---

Here is the other thing, has the customer demanded an MSA off of the CMM? How do you know the checking device is capable of this type of a measurement?

---

this is what we need to figure out. I am not running the job but I believe I will sugggest a few of the issues that everyone has mentioned.

 

Thanks to all,

 

Mike