Okuma spindle ramp-up time speed up?

[danielm]

 

Okuma MA4000B.  OSP300MA control...

 

I'm trying to get tapping time down.  The time for the spindle to get up to speed isn't complete before the hole is already tapped.  Is there a variable anywhere to get the spindle to ramp up faster?

 

Thanks in advance.

DM

[huskermcdoogle]

Likely not one that you would want to change.  It would likely affect sync accuracy.  Other than cycle time, is there a reason you need it to go faster?

If you want good reliable fast tapping cycles you will need to go with something like this:

http://www.tapmatic.com/product_line_self_reversing_cnc_tapping_attachments.ydev

They aren't screaming fast, as they max out at 2500rpm, but you don't have any accel/decel in the cycle time either.  It has potential to slash times pretty good if you are tapping at speeds less than that.

[jeff]

15 hours ago, danielm said:

 

Okuma MA4000B.  OSP300MA control...

 

I'm trying to get tapping time down.  The time for the spindle to get up to speed isn't complete before the hole is already tapped.  Is there a variable anywhere to get the spindle to ramp up faster?

 

Thanks in advance.

DM

How fast are you tapping? I found that if you go upwards of 3,000rpm and higher it's not worth it because of that same ramp up and down time.

[T_MALENA]

On ‎4‎/‎25‎/‎2018 at 7:47 AM, jeff said:

How fast are you tapping? I found that if you go upwards of 3,000rpm and higher it's not worth it because of that same ramp up and down time.

Same thought here...depending on TPI  the spindle/feed is at the max accel/decal rate for the machine.

[Colin Gilchrist]

What material are you tapping? You might have better results with a Thread Mill, since at least you won't have to worry about broken taps...

Another thought

1. You have to "Tap Drill" the hole anyway, right?
2. Why not use a "Thriller" - Combination Drill and Thread Mill Tool? That way you can "Drill" the hole, and at the bottom, you can "Interpolate" the thread? Two Operations, one Tool...

[YoDoug®]

On 4/24/2018 at 2:57 PM, danielm said:

 

Okuma MA4000B.  OSP300MA control...

 

I'm trying to get tapping time down.  The time for the spindle to get up to speed isn't complete before the hole is already tapped.  Is there a variable anywhere to get the spindle to ramp up faster?

 

Thanks in advance.

DM

Make sure you have optional parameter 68 bit 0 checked. It is for high-speed sync tapping. 

 

[danielm]

We tried that Doug .  No change.  We're tapping a 5MX1 hole about 12mm deep.  The tap feed starts as soon as the spindle starts and there just isn't enough time for it to get to speed before the tap is already at the bottom of the hole.  RPM is 5000 and it only gets to about 3000.  The problem is 2 fold...that tap can go faster and TMAC cannot monitor for tool breakage unless the spindle is idled out at RPM.

The spindle load hits 24HP as it ramps up.  You'd think that the torque curve would be enough to get it to speed quicker.  Must be the direct drive....not a geared spindle.

I'm not going to try to tweak the power parameters that the spindle control reads.....but I'm tempted.

 

 

[huskermcdoogle]

Seems to me the only thing that could make it better at this point would be a tapping head.

[jeff]

1 hour ago, danielm said:

We tried that Doug .  No change.  We're tapping a 5MX1 hole about 12mm deep.  The tap feed starts as soon as the spindle starts and there just isn't enough time for it to get to speed before the tap is already at the bottom of the hole.  RPM is 5000 and it only gets to about 3000.  The problem is 2 fold...that tap can go faster and TMAC cannot monitor for tool breakage unless the spindle is idled out at RPM.

The spindle load hits 24HP as it ramps up.  You'd think that the torque curve would be enough to get it to speed quicker.  Must be the direct drive....not a geared spindle.

I'm not going to try to tweak the power parameters that the spindle control reads.....but I'm tempted.

 

 

I have been in the habit of starting all of my taps .500" above the hole to account for ramp up times.

Granted, I don't have hundreds of holes to do, so that extra time is no issue for us.

[danielm]

1 minute ago, jeff said:

I have been in the habit of starting all of my taps .500" above the hole to account for ramp up times.

Granted, I don't have hundreds of holes to do, so that extra time is no issue for us.

 

Wish it wasnt an issue here.  This project is a run off to meet or beat a cycle time.  Right now we are 4 seconds over the time.  Getting the taps to speeds alone would have us under the wire. 

 

[huskermcdoogle]

Look at index position, retract clearance, and toolchanges.  Unless you are doing everything perfect, by combining everything you can, you can likely get your four seconds there.  Moving to and away from the tool change position while the door opens or closes saves a ton of time.  Indexing the pallet on XY approach with a clearance approach in z also helps a ton.

[YoDoug®]

1 hour ago, danielm said:

We tried that Doug .  No change.  We're tapping a 5MX1 hole about 12mm deep.  The tap feed starts as soon as the spindle starts and there just isn't enough time for it to get to speed before the tap is already at the bottom of the hole.  RPM is 5000 and it only gets to about 3000.  The problem is 2 fold...that tap can go faster and TMAC cannot monitor for tool breakage unless the spindle is idled out at RPM.

The spindle load hits 24HP as it ramps up.  You'd think that the torque curve would be enough to get it to speed quicker.  Must be the direct drive....not a geared spindle.

I'm not going to try to tweak the power parameters that the spindle control reads.....but I'm tempted.

 

 

That sounds about right from my experience. That is only 14-15 revolutions of the spindle to reach 3000 rpm. That is quite a bit of acceleration. The bigger the spindle and power, the bigger the mass . The result is slower ramp up time. Okuma's are actually one of the faster machines to go from 0 to full RPM. As far as Tmac, tap monitoring is different than regular monitoring. It requires you to set up a "time slice" of the tapping power to isolate between cutting and ramp up. If the spindle is ramping the whole way you may not be able to use TMAC. 

[YoDoug®]

5 minutes ago, danielm said:

 

Wish it wasnt an issue here.  This project is a run off to meet or beat a cycle time.  Right now we are 4 seconds over the time.  Getting the taps to speeds alone would have us under the wire. 

 

Have you seen the recent video that Okuma put together for cycletime reduction techniques in horizontals? Ask your distributor for a copy of it. It gives a few parameters and techniques that are not readily known. One is how to index the B axis while the machine is tool changing.

[danielm]

5 minutes ago, huskermcdoogle said:

Look at index position, retract clearance, and toolchanges.  Unless you are doing everything perfect, by combining everything you can, you can likely get your four seconds there.  Moving to and away from the tool change position while the door opens or closes saves a ton of time.  Indexing the pallet on XY approach with a clearance approach in z also helps a ton.

We've turned off confirmation for pretty much everything and have the tool door open at tool retract and coolant off.  

[jeff]

10 minutes ago, danielm said:

 

Wish it wasnt an issue here.  This project is a run off to meet or beat a cycle time.  Right now we are 4 seconds over the time.  Getting the taps to speeds alone would have us under the wire. 

 

Any other ops that you can shave time off of? Drilling maybe? No spot?

Eliminate a tool change and there's your 4 seconds. Without seeing your current parts and how it runs we can only just give you guesstimates. 

[huskermcdoogle]

Just now, danielm said:

We've turned off confirmation for pretty much everything and have the tool door open at tool retract and coolant off.  

Are you retracting all the way to z home for tool change, if you are, change it so that you are only retracting as far as you need for the longer of the two tools involved in the tool change.  If you have more than 4 tool changes, you should get your four seconds.

[danielm]

21 hours ago, Colin Gilchrist said:

What material are you tapping? You might have better results with a Thread Mill, since at least you won't have to worry about broken taps...

Another thought

1. You have to "Tap Drill" the hole anyway, right?
2. Why not use a "Thriller" - Combination Drill and Thread Mill Tool? That way you can "Drill" the hole, and at the bottom, you can "Interpolate" the thread? Two Operations, one Tool...

 

Will check that out Colin!  Thanks!!

[danielm]

15 minutes ago, YoDoug® said:

Have you seen the recent video that Okuma put together for cycletime reduction techniques in horizontals? Ask your distributor for a copy of it. It gives a few parameters and techniques that are not readily known. One is how to index the B axis while the machine is tool changing.

 

I'll lok for that Doug.   Thanks!

[huskermcdoogle]

21 hours ago, Colin Gilchrist said:

Why not use a "Thriller" - Combination Drill and Thread Mill Tool? That way you can "Drill" the hole, and at the bottom, you can "Interpolate" the thread? Two Operations, one Tool...

My only experience with these is in cast aluminum.  They are a huge time saver if you only have a few shallow tapped through holes per part, and don't have too many parts on the table.  Given an application where they fit, they will shine.  I have never used them in a blind application, but if the design will allow for it, I would imagine they will do great.

 

What other features do you have to play with on the part?