What's new
What's new

# Drill time from hole to hole

#### Motorsports-X

##### Hot Rolled
I seem to remember doing something like this in school, but its been so long. I havent drilled this many holes in a while.

I have some plates with holes, about 3000 total. is there a way to make the machine move in an ark from hole to hole instead of horizontal/vertical movements? (think sine wave vs square wave) Im mainly interested in doing this for the spot drill.

#### DMF_TomB

##### Diamond
I seem to remember doing something like this in school, but its been so long. I havent drilled this many holes in a while.

I have some plates with holes, about 3000 total. is there a way to make the machine move in an ark from hole to hole instead of horizontal/vertical movements? (think sine wave vs square wave) Im mainly interested in doing this for the spot drill.
.
some CAM programs you can select moving to position 1 axis at a time. moving x and y at same time or moving xyz at same time

#### Finegrain

##### Diamond
Not sure I understand what you're trying to accomplish. Feed plane should be just a tad above the work surface so I don't see how arcing would make any measurable difference. In X & Y, surely your control takes you in a straight line from Point A to Point B, no?

Regards.

Mike

#### Matt@RFR

##### Titanium
What machine? Is this one of those old turds that like to stop and pause for 8 minutes at every direction change?

If you're on one of them Haas turds: It could be as simple as turning setting 57 "Exact stop canned X-Y" off. At 100% rapid it'll pretty much make an arc like you're talking about, just make sure you have your clearance height high enough. Not sure it will actually help your cycle time though.

#### 2outof3

##### Titanium
Not sure I understand what you're trying to accomplish. Feed plane should be just a tad above the work surface so I don't see how arcing would make any measurable difference. In X & Y, surely your control takes you in a straight line from Point A to Point B, no?

Regards.

Mike

In many older controls, the control change from feed to rapid is accompanied with some thinking time. This is about servo control loop speed.

#### 3t3d

##### Diamond
There is an option like that in the Robodrills, and I assume by association, other Fanuc controls.

Basically what you describe is how I interpreted the explanation... It starts and stops the X,Y motion without having the Z get to an Exact stopping point.
Intended for speeding up the hole to hole time.

#### Motorsports-X

##### Hot Rolled
This is on a haas tm2

3t3d your right... That's where i saw it at before. I don't guess the haas can do it. Like someone said above though, rapids with setting 57 off might do it

#### AARONT

##### Stainless
You could try setting 247, but I believe it is only on tool changes.

"Setting 247 is a control feature that requires the Z Axis to move to the tool change position first, followed by the X and Y Axes. If Setting 247 is OFF, the Z Axis retracts first, followed by X- and Y-Axis motion. This feature can be useful in avoiding tool collisions for some fixture configurations. If Setting 247 is ON, the axes move simultaneously. This may cause collisions between the tool and the workpiece, due to B- and C-Axis rotations. It is strongly recommended that this setting remain OFF on the UMC-750, due to the high potential for collisions."

#### Vancbiker

##### Diamond
Mits controls have available "high speed canned cycles". Use of I and J addresses in the canned cycle control the amount of "arcing" into position. I played with it a bit on my machine but in a 10 hole test program, I could not measure any time savings. Not really a surprise on a machine with over 1900IPM rapids and quick accel/decel times though.

#### deljr15

##### Cast Iron
If setting 57 does not fix your problem you could use a macro to handle the drilling instead of the canned cycle.

#### Motorsports-X

##### Hot Rolled
Never done anything with macros...

#### Needshave

##### Aluminum
I think the best way to reduce cycle time would be to use as few tools as needed. We use some drills by Mitsubishi that run with no spot and no peck. If you have a call out for a counter sink you could get a special made to machine it with the same tool.

#### 706jim

##### Stainless
While not exactly what is being asked here, I thought I would make a comment. Many years ago around 1976, we bought a Whitney punch press with a GE 550 control. It would punch holes along a planar arc, and as was typical with many older controls, this was limited to a max arc of 90 degrees.

So, when presented with a speaker grill job with holes defined on arcs, I gave it a try. The end result was that while it worked and the holes ended up where they were supposed to be, it was a LOT more work figuring out the arc distance between successive holes every 90 degrees and on several different radii.

#### 2outof3

##### Titanium
So much more to drilling holes when they are small and there are thousands. Tool life is a big issue and this leads to better spindles versus other factors. If I was trying to do this on a TM I definitely would stay away from carbide. Do you have a tool setter to check the drill to make sure you don't spend hours cutting air in a ruined part. Servo and servo lag will lead to the proper timing of the time to start the actual drill cycle. I like the idea of staying in feed mode instead of going from feed to rapid back to feed. Also if the drills are small, sometimes the speed of the movement can fracture the drills.

I have a customer who has to drill thousands of holes per part. The same part, with the same program can run over 20 hours on one of his machines and under 12 hours on another. Same tools, same RPM, same program but different machines with different controls.

This is a bit of an art form where experience matters.

#### Motorsports-X

##### Hot Rolled
I'm doing acrylic. I wouldn't do steel on the tm. I found some acrylic drills for \$14 that I'm Using, and a diamond em for the counter bores (full depth circle interp., about 4-5 seconds per hole.)

#### 2outof3

##### Titanium
I'm doing acrylic. I wouldn't do steel on the tm. I found some acrylic drills for \$14 that I'm Using, and a diamond em for the counter bores (full depth circle interp., about 4-5 seconds per hole.)

Watch your coolant. Fine acrylic turns into oatmeal.

#### Finegrain

##### Diamond
I'm doing acrylic. I wouldn't do steel on the tm. I found some acrylic drills for \$14 that I'm Using, and a diamond em for the counter bores (full depth circle interp., about 4-5 seconds per hole.)

Have you considered plunging an endmill for most of the counterbore? That would be fast, and make 4 strings instead of a zillion tiny plastic bits.Get or have made an endmill .005" undersize, and plunge it within .005", then finish with your EM.

Regards.

Mike

#### Motorsports-X

##### Hot Rolled
I have considered, and attempted that in the past. I wasnt happy with the finish. This way takes longer but I'm happier with the end product, and a vacuum takes care of the chips easily

#### Motorsports-X

##### Hot Rolled
I should of read your post more Carefully.. I didn't think any the undersized endmill part. That's not a bad idea

#### G00 Proto

##### Hot Rolled
I agree that the Haas canned cycles for drilling leave something to be desired. It seems like the machine spends an excessive amount of time thinking about each hole before it gets down to business. I used to make plates with thousands of complex holes in them. Materials ranging from ground 7075 to 6Al4V. I dicked around with bunches of different tool path strategies to try and decrease cycle times. I even wrote one program that spot drilled and drilled on rapid, no canned cycles. It was a joy to behold... 10,000 RPM and G00 into the hole. Chips came out like high velocity lances. Ran like a raped ape until the shop owner came by and gave me the WTF speech. But I digress.

The only way I substantially impacted the profitability was by getting custom ground step drill. In other words, without seeing you part, it sound like you need a stubby carbide tool that has a drill portion, and counter bore section... since you are getting it custom ground, I always put in edge breaks as well for the top of the hole and the counterbore to hole junction. Then it is one tool that makes a finished hole. They used to cost me about \$150, and took a hole that took 4-5 drill cycles down to one. Then we were printing money. Well actually the boss was printing money... I was using the extra time to polish my resume.

Replies
23
Views
1K
Replies
9
Views
740
Replies
14
Views
1K
Replies
28
Views
1K
Replies
4
Views
202