Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Drill P20 with HSS drills


Recommended Posts

I don't use a calculator... 70-100 sfm using HSS for P20... low side uncoated, spin it a bit faster if coated

 

Feedrate depends on drill size... generally speaking... 1/2" drill, around F4.0 ipm, less the smaller you go because of flute clearance... less the bigger you go because of horsepower limitations... of course, you want  a good sharp drill to start, and the chips are a good indicator of proper speed/feed... flood coolant and peck... chips should be a nice shade of brown... not blue... hth

Link to comment
Share on other sites

Good afternoon

 

Does any one know a good online speed and feed calculator for

drilling P20 with High Speed Drills 5- 8 inches deep?

 

Our shop has moved on to also making P20 steel molds now and

I have only made a few Cast Iron Molds many many years ago.

 

Any help will be greatly appreciated

 

Cheers

rick

 

I'm more conservative than Reko. For P20 with HSS tools;

 

50-60 SFM and 1.2% to 1.5% of the drill diameter per rev feed.

 

+1 million on the Titex tools assuming you're talking about through cool. We've got some Titex drills but are very well stocked with Mitsubishi high performance drills. The machines we drill on all have 1000psi through tool cooling. example: high hard P20, 1/2" water lines (.720 drill) 7" deep. No spot drills, no pecks, slow feed in half while intersecting two cross holes = 35 seconds each.

  • Like 2
Link to comment
Share on other sites

For a 1/2" HSS uncoated HSMAdvisor is recommending S260 F1.87 (34SFM, .00144IPT) with a .25" peck.  If I go to cobalt it says S313 F2.25 (41SFM, .00144IPT).

Speeds and feeds at 100% on HSMAdvisor are considered uber-safe conservative.

150% on speed and feed will move you close to what many manufacturers suggest.

Link to comment
Share on other sites

For a 1/2" HSS uncoated HSMAdvisor is recommending S260 F1.87 (34SFM, .00144IPT) with a .25" peck.  If I go to cobalt it says S313 F2.25 (41SFM, .00144IPT).

 

i've been carving molds out of P20 for 1/4 of a century therefore my experience trumps HSMAdvisor. :cheers:

 

 

leave. it. alone. , Reko! :lol:

  • Like 2
Link to comment
Share on other sites

I'm more conservative than Reko. For P20 with HSS tools;

 

50-60 SFM and 1.2% to 1.5% of the drill diameter per rev feed.

 

+1 million on the Titex tools assuming you're talking about through cool. We've got some Titex drills but are very well stocked with Mitsubishi high performance drills. The machines we drill on all have 1000psi through tool cooling. example: high hard P20, 1/2" water lines (.720 drill) 7" deep. No spot drills, no pecks, slow feed in half while intersecting two cross holes = 35 seconds each.

 

How do you get your program to slow down during cross lines?  Do you have a special post mod for that?  Our operators just slow the drill down for the entire cycle.

Link to comment
Share on other sites

How do you get your program to slow down during cross lines?  Do you have a special post mod for that?  Our operators just slow the drill down for the entire cycle.

 

i program manually and run them as sub programs when doing multiple locations. having full control over parameters is even more important for deep holes (15, 20, 25, 30X dia) when you need to enter the pilot holes slowly then turn the coolant on and ramp the speeds and feeds up to cutting speeds, drill, then rapid back to the start point and slow the speeds and feeds back down to retract out of the holes.

 

i've been tempted to write a post mod or macro, but meh, it's easier to write a few lines of code for drilling manually.

Link to comment
Share on other sites

i've been carving molds out of P20 for 1/4 of a century therefore my experience trumps HSMAdvisor. :cheers:

 

 

leave. it. alone. , Reko! :lol:

That is what i like to hear.

 

i used this info and got through the drilling no problem

 

Next question for Roughing.

 

I am awaiting on a 2" high feed cutter(Eta 1hr) i'll get exact details shortly

 

Looking for speeds, feeds, DOC and Step over.

 

I have to design and program 4 or 5 on graphite molds while i keep this P20

progressing.

 

I apologize for late replies as i am on 14 hr shifts of madness....LOL

 

Thanks in advance for all help.

 

When I get through this job it will start a new avenue of p20 permanant mold

and casting at our shop

 

I greatly appreciate Everyone help

 

BTW I am cutting the cavity first so all the major drilling is on the Core base which i will hopfully

start at the end of next week

 

 

About 3" reach on the cutters for this cavity

 

36" x 32" x 8"

 

.

cav%20p20_zpshmphyder.png

Link to comment
Share on other sites

depths of cuts will depend largely on tool geometry and machine horsepower. we use ingersoll and mitsubishi high feed mills. the ingersoll's can go to .025 doc, the mitsubishi's up to .05 doc.

 

500-600 SFM , .025 to .03 chip load is a good place to start. air blast for cooling. 70-75% of the tool (effective cutting) diameter stepover, or less if you can't get Mcam to not grow random islands while roughing which will easily banzai the tool in materials like P20.

Link to comment
Share on other sites

that's a reasonable starting point i think, 900rpm at 120ipm. though the doc might be a little heavy due to there not being much rake on the inserts. your machine will quite likely let you know right away whether or not it's happy. use generous toolpath radii to keep it out of sharp corners. have fun. :thumbsup:

Link to comment
Share on other sites

Cool, thanks a ton!

 

It seems happy, although this is an old non-rigid VF6 so the spindle load is

jumping around over 100%

 

I increase the RPM to 1050 , seems happier... ;)

 

This machine has a brand new spindle as of a month ago. :)

 

I am using a .625 entry helix, seems ok

 

Might have to cut the feed down a bit....mayberto 100ipm

 

and my bosses are trying to talk me into lights out for the entire path on

one set of inserts....14hr path...i shake my head when they get involved......

 

I programmed to 1" deep, I will watch it untill the inserts give out

see what level i am at and program 80% total depths at a time.

 

Cheers

Link to comment
Share on other sites

lights out? high feed? P20? we wouldn't even do that on the big horizontal where gravity takes care of the chips.

 

i program tool retracts (spindle + cooling off / z axis home / program stop) for insert inspection (tool inspection / change feature on tool param page in Mastercam) for every 30 minutes to deal with chips and check inserts. 1.5 to 2 hour insert life is fairly conservative. 45 minutes to 1.25 hours is fairly aggressive. in my opinion. all night? no freakin' way! ymmv.

Link to comment
Share on other sites

lights out? high feed? P20? we wouldn't even do that on the big horizontal where gravity takes care of the chips.

 

i program tool retracts (spindle + cooling off / z axis home / program stop) for insert inspection (tool inspection / change feature on tool param page in Mastercam) for every 30 minutes to deal with chips and check inserts. 1.5 to 2 hour insert life is fairly conservative. 45 minutes to 1.25 hours is fairly aggressive. in my opinion. all night? no freakin' way! ymmv.

Update

 

i told them not to dream any more and let me and the skilled colleages

that are helping me get through this.....

 

Just stopped it to get the chips off the way at back of machine

 

i was at z level -.175 bout half way through the lvl

 

I checked the inserts, would have just made it through that level

 

So, that is my number and i will program .175 at .035 DOC for each insert change

 

Cheers

  • Like 1
Link to comment
Share on other sites

Time to get those carbide inserts into the wire machine and give them a new edge.  Yes I have seen this done.  It's insane and pointless and a huge waste of money and time but when your boss is really really cheap that's what you get.

If you are using DME's P-20 base I would use extra caution on drilling.  For the last 3 years or so that steel has had quite a bit of hard spots.  It's also a huge pain when machining small detail in core and cavities.  

Link to comment
Share on other sites
  • 3 years later...
On 6/2/2016 at 1:47 PM, Mjölnir said:

lights out? high feed? P20? we wouldn't even do that on the big horizontal where gravity takes care of the chips.

 

i program tool retracts (spindle + cooling off / z axis home / program stop) for insert inspection (tool inspection / change feature on tool param page in Mastercam) for every 30 minutes to deal with chips and check inserts. 1.5 to 2 hour insert life is fairly conservative. 45 minutes to 1.25 hours is fairly aggressive. in my opinion. all night? no freakin' way! ymmv.

resurrecting this topic.  Is a post mod needed to achieve the above statement? TIA

 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...