HSM question ???

[mastercamguru]

I would like to introduce HSM to my shop, but I want to have "dead on"(or as close as possible) speed/feed & axial/radial doc parameters to start with, before presenting this to the owner. It seems a shame that Mastercam has these new HSM features, but no parameter info.

Is there any method or software available to help me bring this shop up to speed?

[tobyaxis]

Mastercamguru there's Tons of info on HSM online alone.

Here is some to get you started.

http://books.google.com/books?id=Ccj...ng&lr=#PPP1,M1

http://books.google.com/books?id=Zbm...peed+Machining

http://www.datrondynamics.com/high_speed_machining.htm

http://02c9c5d.netsolhost.com/samples.htm


BTW: got your message, but can't call back till around 7:30pm. Have a bit of work to finish.

TTYL

[mastercamguru]

That's ok....I was in the middle of writing a macro program. Always taking work home... I'll check these links out meanwhile.



Powered by:

[mastercamguru]

Toby:
I keep missing you, but that's OK....I'm ready for a test run tomorrow (yeah I work Saturday too) with RobbJack's parameters "plugged in". They are almost the same as Mastercam's HSM defaults. I just hope the control can keep up with the code. I'll start at 120ipm and ramp up to 240ipm (my machine's limit) to see if feedrate drops due to processing time at the control. If I hit a "ceiling" or feedrate limited by the control, I'll comp with a bigger step-over % to make a respectable MRR............Wish me luck.




Powered by:

[tobyaxis]

HSM doesn't mean that you have to go 1000IPM LOL.

Your best bet is to find out what the Maximum feed rate is in the machine manual. Start your tool at the Maximum Programmable Feed and Speed. Set your Feed Over Rides at 25% and let her RIP!!!!

Tool Max Depth should fall around 25% of the Diameter at about 75% Max Width.

Example:

Machine Hardinge VMC XV710
CAT 40 Spindle
8,000 RPM
400 IPM

Tool 1.0 SECO TURBO MILL 1/32 CR 3FLT POLISHED INSERTS
Material Aluminum 6061-T6
Rigid Set-Up

This machine usually hits a Max of 8000 RPM, 380IPM, .15 DOC, .75 WOC.

Gets a bit smokey with the coolant evaporation but it cuts NICE!!!!!!

I received your message a little late in the evening. LOL the little woman kidnapped me for more shopping. She buys, I load the truck and carry. One starts to wonder if this was in the original contract of being in a relationship.

I'll try you back today.

[mastercamguru]

Toby:

That was just about "dead on".

My machine manual says the max feedrate is 240ipm, but I can get 393.7ipm, so 380ipm
is an ideal # for a max value. My Walter insertable with polished APKT inserts .03 rad cut nice with your numbers. Thanks for the help with a documented starting point. Now I can start a specific tool library for HSM, so I'm not guessing, and I can be confident that I won't be creating problems.....eg. melting our nice brand new insertables....and I'll be ready to make respectable MRR's when we get a new Horizontal. I'll be testing out RobbJack's new line of EM's specifically suited for HSM.(A-1 & FM series)

I now know that I can "cut" with these faster parameters, but now I lose accuracy in corners (control moves next axis before current axis reaches position).

I understand this is what is known as "servo lag". I tried out "exact stop mode" G61, and it cleaned the corners, but also dwelled in cornering, defeating the HSM method. So I found a "work around".

After reading into AI-nano and Mazak G61.1 modes, I found my answer. Mazak G61.1 factors the feedrate in corners. If I emulate this behavior in my post I now have G61.1 (sort of).LOL

Here's what I did:

#[misc reals]
#         1. "G13 - Plunge Feedrate"         
#         2. "G13 - Roughing Feedrate"      
#         3. "G13 - Finishing Feedrate"     
#         4. "G13 - Rapid Feedrate" 
#       
#         5. "Arc Feedrate Factor"  <--------multiplies feed by this value
#         6. "Arc Threshold"  <--------------if arc rad falls below this value
#
#         7. "Output Toolpath Subs? [0=No, 1=Yes]"
#         8. "How Many Offsets? 1-6"                          
#         9. "G13 - Clearance Plane"  
#         10. "G13 - Feed Plane"  



pcirout1        #Output to NC of circular interpolation
      pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,
        pxout, pyout, pzout, pcout, parc,
        [                        #<-------------------------here
         if arcrad$,
         [if arcrad$ <mr6$ & arcrad$ >-mr6$ & mr5$<>0,feed = feed*mr5$]
        ],
        if feed <0.01,feed = 0.01
    feed, strcantext, scoolant, e$    #<-------------------------to here

This is working fine for now, as long as there is an arc move in the corner.

Any ideas for another option to emulate this feedrate control for linear moves?

Is there an option in high speed toolpaths to do this for linear moves?







Powered by:

[Mike Mattera]

Have you ever played with the High Feed option? It will increase/decrease your feed for changes in direction and volume of cut. It has options for deceleration on corners.

Mike Mattera

[tobyaxis]

Originally Posted by mastercamguru Toby: That was just about "dead on". My machine manual says the max feedrate is 240ipm, but I can get 393.7ipm, so 380ipm is an ideal # for a max value. My Walter insertable with polished APKT inserts .03 rad cut nice with your numbers. Thanks for the help with a documented starting point. Now I can start a specific tool library for HSM, so I'm not guessing, and I can be confident that I won't be creating problems.....eg. melting our nice brand new insertables....and I'll be ready to make respectable MRR's when we get a new Horizontal. I'll be testing out RobbJack's new line of EM's specifically suited for HSM.(A-1 & FM series) I now know that I can "cut" with these faster parameters, but now I lose accuracy in corners (control moves next axis before current axis reaches position). I understand this is what is known as "servo lag". I tried out "exact stop mode" G61, and it cleaned the corners, but also dwelled in cornering, defeating the HSM method. So I found a "work around". After reading into AI-nano and Mazak G61.1 modes, I found my answer. Mazak G61.1 factors the feedrate in corners. If I emulate this behavior in my post I now have G61.1 (sort of).LOL Here's what I did: #[misc reals] # 1. "G13 - Plunge Feedrate" # 2. "G13 - Roughing Feedrate" # 3. "G13 - Finishing Feedrate" # 4. "G13 - Rapid Feedrate" # # 5. "Arc Feedrate Factor" <--------multiplies feed by this value # 6. "Arc Threshold" <--------------if arc rad falls below this value # # 7. "Output Toolpath Subs? [0=No, 1=Yes]" # 8. "How Many Offsets? 1-6" # 9. "G13 - Clearance Plane" # 10. "G13 - Feed Plane" pcirout1 #Output to NC of circular interpolation pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia, pxout, pyout, pzout, pcout, parc, [ #<-------------------------here if arcrad$, [if arcrad$ <mr6$ & arcrad$ >-mr6$ & mr5$<>0,feed = feed*mr5$] ], if feed <0.01,feed = 0.01 feed, strcantext, scoolant, e$ #<-------------------------to here This is working fine for now, as long as there is an arc move in the corner. Any ideas for another option to emulate this feedrate control for linear moves? Is there an option in high speed toolpaths to do this for linear moves? Powered by:

How crafty of you to find this. Good Work MCGURU Your a true craftsman!!!!!!!!!!!