Incorrect drilling?

[chunkstyle]

Bought a couple of brad point bits in 1/8" and 5mm sizes from vortex. Wanted to see how they would do for pilot hole drilling and system hole drilling using my spindle.

1/8" is set up as tool #14, .125" D, 3k spindle speed, max. penetration .5". Drill type an is operation #1.

5mm bit is set up as tool #15, 5mm D., 3k spindle speed, .375" max penetration, Type: drill, Operation #2.

.25" M.C. bit for all the rest of the cutting.

Output the file to SB and run the first sheet. (no more bit slamming into material : ). SB3 calls up tool #3 correctly and proceeds to drill out all the holes on the sheet, INCLUDING 5mm system holes!

I've been looking around in the link settings to see where something might be out of place but everything looks in order. Anyone have an idea on what to check for this problem?

Thanks,
Tim

[chunkstyle]

Tried using the "Interpolate" for both bits. Set their max Interpolate to .125" and 5mm respectively. Just re-ran the file and it's still using the .125"D bit to drill 5mm system holes.
Tolerance is set to .01"

[chunkstyle]

Tried changing the max. interpolation .01" over bit both drill bit diameters and reloaded the file.
No change. Uses first bit for all hole drilling.
Looked thru the code and there doesn't appear to be any call for a tool change anywhere in the file for all the drill operations on this sheet.

[chunkstyle]

Anyone use two different size drill operations in the same sheet and have the Link call up the tools correctly?

Not asking for instruction . I just want to know that it can be done and has been before I try and sort it out with Thermwood on Monday.

Thanks,
Tim

[Gary Campbell]

Tim...
First...When using drill bit, tool settings must be drill only. Interpolation is NOT an option. This is only used for a router bit, say for example, 1/4" to bore a 3/8 hole.

Try this:
Set your largest bit (5mm) as operation #1
5K rpm, 120 ipm plunge .197 diameter tool # 15
max pen to .8
CHECK DRILL ONLY (uncheck all others)

Set your 1/8 bit as operation #2
5K rpm 120 ipm plunge .125 dia, tool # 14
max pen to .8
CHECK DRILL ONLY (uncheck all others)

Set your tolerance to .005
Rerun file

Last question: What is tool# 3 you mention?

The reason a tool change is not called for is that you have your parameters set to allow (or force) the 1/8 bit to drill 5mm holes.

[chunkstyle]

OOOOPs! Typo Gary. Meant tool #14. Sorry for confusion.

I'll do just as you say. Should I assume that the drilling needs to be set up from larger to smaller?

Thanks alot. Been working at getting the machine to work so I can get to work all day.

Tim

[Gary Campbell]

Tim...
When setting up tooling operations, ALWAYS list bits from largest to smallest.(drills and end mills) This forces the largest bit possible to cut a given geometry

[chunkstyle]

Thanks Gary,

Great to have you out there doing what it is you do. Yet one more time you got my machine plugged in and pointed in the right direction.

Machine's cutting and were making dust again.

Thanks heaps,
Tim

[Gary Campbell]

Tim...
Since we have been talking about backups and saving files, here is another tip for you: Once you have your SB Link settings where you want them, do an export and name the file something like, "TM Link Settings.cab"

Should you fry your computer, lose the existing settings, or simply want to transfer those settings to another computer, just import that .cab file, and you are up and running.

Same goes for SB3. Click on [U] [S] and save the existing SB3 settings to a file that can also be used to restore or move settings to another computer.

SB3 has been getting more and more fickle over the last 20 versions. Being able to install "known working" settings after lost comm, lost position, erroneous or real stop hits, power surges or computer malfuntions is imperative to the guy who needs the machine to make a living.

[MogulTx]

Gary,

Thanks for the insight on the tool and size sequence opinion. I can see why that would be well advised, but it had not really reached the level of "realization" yet for me. I should use the largest bit possible because it will have greater surface area, and should run cooler while taking bigger cuts- as long as it is small enough to get into the geometry to do the job... I have not set up an "orderly method" of attacking a job. My sequence has been (1) holes or through diameters, (2) partial pockets to X depth and then (3) all severing cuts (peripheral cuts for components).

I am going to go back and study the back up suggestiuons you posted also. I have an XP box that only has 512M RAM, and I want to update/upgrade that. I did not set up any of the parameters on this- and would be lost if I had to duplicate it on another machine if a failure should occur. I think I should also go to NC and do an in-house class so I can pick up some of the formal training that I did not get by buying a used machine. I am doing pretty well, and figuring things out, but there is no sense in struggling through it if I don't have to- and guys like yourself are APPRECIATED for your input. Believe Me.

Thanks. Many times over.

Monty