aligning cross holes

[hacdlux]

i just got done doing a prove out on a part that by necessity has to have a coss hole drilled on the main then c'bored and reamed in the sub

i drilled the pilot then indicated it in the sub then fine tuned with test cuts

my problem with this whole process is if you junk an insert any where in the part you have to start the process all over

oh, machine is a tsugami ss32
part is 316ss
tolerance on hole is .001 tp, .0002 dia .00008 roundness

im really just looking for better idea on how to manage the offsets particualrly my cutoff/ grooving insert, that is the one giving me the most headache

[ProProcess]

i just got done doing a prove out on a part that by necessity has to have a coss hole drilled on the main then c'bored and reamed in the sub

i drilled the pilot then indicated it in the sub then fine tuned with test cuts

my problem with this whole process is if you junk an insert any where in the part you have to start the process all over

oh, machine is a tsugami ss32
part is 316ss
tolerance on hole is .001 tp, .0002 dia .00008 roundness

im really just looking for better idea on how to manage the offsets particualrly my cutoff/ grooving insert, that is the one giving me the most headache

A few questions....

Why do your cut-off and grooving inserts have an effect on the location of your cross holes?

To me, holding that type of positional tolerance with a reamer in the sub that is going into a hole that was drilled on the main, sounds like a loosing battle.

Is there any other way to process the part?
Can you post a picture or print?

[gizmo_454]

A few questions....

Why do your cut-off and grooving inserts have an effect on the location of your cross holes?

My "assumption" here is that maybe he is using the grooving tool as the cutoff and when it wears out, it deflects enough to change the location of the cross drilled hole in relation to some mystical point on the part.

To me, holding that type of positional tolerance with a reamer in the sub that is going into a hole that was drilled on the main, sounds like a loosing battle.

Having limited experience with swiss type machines, (about a year), I have to ask: Why does this sound like a losing battle? Our E32 Citizen, even being 17/18 years old, does not have issues holding locations between main and sub. Why would a new SS32 Tsugami?

Is there any other way to process the part?
Can you post a picture or print?

A print or picture would definitely be nice...

Mike

[SirDenisNayland]

I am also not familiar with this particular machine but ill take a stab at deciphering what he means.

He says he had to dial in the sub, I'm guessing to find the c axis value for the correct orientation. If an insert is scrapped and the job has to be reset then he loses that position.. I would think the machine can phase the main and the sub to where this wouldn't be an issue, but this is the only thing I can think of. I've had to dial in on hex before and if the bar failed to load for whatever reason id have to redial it.

It's not optimal to be splitting aspects between the main and the sub because it allows just that much more room for positional errors. With the tolerances he describes he has to be NUTS on. It will make the part yes, but it makes it that much harder to make to spec... Especially if you're constantly having to redial it in.

If anything is off even the slightest it causes a cascading error. Say your sub spindle is a few tenths off, say the spindle sync is slightly less than stellar, say if you are forced to use very low chucking forces which could potentially cause a slight spin of the part, part flex in the sub, a tiny tiny chip getting stuck throwing the concentricity of the part and the spindle off by as little as a few tenths etc. When you're holding plus minus 5 degrees and you have a few thou of tolerance and run out its easy to forget about these tiny details that can make or break a part with much more stringent tolerances. Also sometimes there are the anomolies or gremlins we all know and love that make things difficult for no apparent reason at all.

I think the real issue is his theblife of his cutoff and groove tool here, not so much the part. As he said its a necessity to make it the way he is doing it.

[hacdlux]

sorry guy its been a busy week

unfortunatelly cant post a print

the cross hole is at the rear of the part and has a setscrew coming in through the rear face

i drill the cross hole on my main
then in the sub
drill and thread the set screw
then cbore and ream the cross hole

my tool zone is similar to this

2 cross tools in the rear and i need 3 for the feature


if i finish out the hole on the main then try to do the set screw it will ruin the cross hole



the problem i was having is im using my cut 31 cutoff blade to do some roughing behind a shoulder so if i adjust how much material is on the shoulder it changed my cutoff position

changing where my pickoff was moved the cross hole in relation to my cross reamer in the sub

i think when i go into production i will use 2 different tools so my cutoff will remain consistent

[gizmo_454]

There is probably a reason, so this is probably a dumb question... Without seeing a print/chicken scratch/description, it's hard to understand what the part looks like. Can you run the part with the "set screw" and "counter bored/reamed" cross hole on the main and do the other end in the sub? Basically, flip the part end for end.

Mike

[ProProcess]

... my tool zone is similar to this

2 cross tools in the rear and i need 3 for the feature...

maybe not...
It appears that maybe you have Y axis in the back?
If so, you could use G2/G3 and mill the hole close to size in the back, then ream so finish size.
Just a thought.

[MCImes]

First thought: Add a back turn tool. Thats the best solution if you have an open tool.

If you cant add real back turn tool to your setup I often put the same tool on different offsets to control different features. So do your cutoff with T0101 and your back turning with T0131 or something like that.

I do this often when I mill flats that are far apart. For some reason the milling at the back of the part usually has a -.006 difference from the front so I just touch off my endmill in tool 1 then put the same # in geometry offset for a fake tool (like offset 31) and then I can control the features separately in x and z. using your tolerance doesn't get you very far when you have +0 -.001.

Try that?