1. This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn More.
  2. PLEASE: Read the FORUM RULES BEFORE registering!

    Dismiss Notice

Ramp Vs Spiral Vs Plung Lead-in Technique

Discussion in 'CNC IN THE HOME SHOP' started by Boswell, Aug 27, 2016.

Tags:
  1. Boswell

    Boswell United States Hobby Machinist since 2010 H-M Supporter-Premium

    Likes Received:
    83
    Trophy Points:
    28
    City:
    Cedar Park
    State:
    Texas

    -Return to Top-

    I would like to hear opinions on the use of RAMP, SPIRAL and PLUNG as lead-in to interior pockets. I have almost exclusively used the Spiral technique mostly due to small pockets with limited space but recently I have been working on parts with large interior pockets and started wondering what advantage (if any) using a Ramp technique would have. Plung does not seem very practical unless there is no choice because it is so hard to clear the chips from the cutter. Plung might make more sense if I had a high velocity flood coolant delivered through the tool but I only use a Fog Buster type.

    Thanks for your thoughts on this?
     
  2. T Bredehoft

    T Bredehoft Active User H-M Supporter-Premium

    Likes Received:
    1,025
    Trophy Points:
    113
    Location:
    Central Ohio
    City:
    St. Louisville
    State:
    Ohio

    -Return to Top-

    I used a spiral ramp, leaving stock on the side of the "bore,", then changed the cutter diameter for a final pass. I'd written sub-routines for these where I just filled in depth of finish cut diameter and tool no.
     
  3. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    366
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    I u
    I have used ramping only because my CAM program (D2NC) won't do it any other way. It works OK but there have been instances where I would have liked to have a choice. Just bought CamBam and still learning what it can do. It has spiral, tangent and plunge pocketing and profile capability. I really like the tangent option. It allows you to set a lead out radius rather than having to manually tweak the code to run the cutter off the end of the part. I avoid plunging if at all possible for the reasons you gave and also because it's hard on the cutter.

    Tom S.
     
  4. Boswell

    Boswell United States Hobby Machinist since 2010 H-M Supporter-Premium

    Likes Received:
    83
    Trophy Points:
    28
    City:
    Cedar Park
    State:
    Texas

    -Return to Top-

    thanks. I should say that I have been using BobCad for a while now and overall have been very happy with it as a CAM system. Not so much as a CAD system though and still use Autocad for drawing. For profiling, where I can approach the work from the side, BobCad also allows me a number of options.
     
    TomS likes this.
  5. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,335
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    When I have to plunge in a pocket, I normally drill a hole where the plunge will occur. Normally the first operation is to drill all the holes in the work, so this doesn't require an extra operation. Generate the tool path first, then add a circle at the cut start point(s), put it in the drill operation, and regenerate the tool paths. Where possible, set up a plunge off of the part, cutting air is really easy on the tool.;)

    I also have CamBam and have found it to be very flexible and easy to torture it into doing things my way. Been using it for about 4 years. Slowly transitioning to Fusion360, but it's painful for me. No problem using the CAM functionality, but I'm having a hard time getting my head around 3D modeling.:confused:
     
    TomS likes this.
  6. RJSakowski

    RJSakowski H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    1,879
    Trophy Points:
    113
    City:
    Barneveld
    State:
    Wisconsin

    -Return to Top-

    The problem that I see with plunging is that the end mill is least efficient at cutting at its center because of the the zero cutting radius. Either ramping or spiraling in eliminates the problem. Spiraling is simply ramping in a circle. They are essentially equivalent in their effect. Which one I use depends on the part. I would use a ramp for cutting a slot and spiral for circular pockets.

    One advantage of a spiral is you are not cutting full depth sidewalls simultaneously as you ramp in.

    In cases where I cannot use either a ramp or spiral entry, I will pre-drill a pilot hole to eliminate the cutting at zero cutting radius.
     
    JimDawson likes this.
  7. Boswell

    Boswell United States Hobby Machinist since 2010 H-M Supporter-Premium

    Likes Received:
    83
    Trophy Points:
    28
    City:
    Cedar Park
    State:
    Texas

    -Return to Top-

    When machining an internal pocket that is large enough that both a Spiral and a Ramp approach will fit the space is there any advantage to one over the other? Is one faster or easier on the tool?

    RJ, good point about a spiral entry will never result in a full depth full slot cut where at the end of a ramp this will be true.
     
  8. tmarks11

    tmarks11 Active User Active Member

    Likes Received:
    176
    Trophy Points:
    43
    City:
    Port Orchard
    State:
    Washington

    -Return to Top-

    Ramp or Spiral will make your endmill last longer.

    As RJ said, when plunging you are engaging the material near the center of the endmill with it turning at sub-optimum speeds, leading to excessive wear.

    I would say spiral is better for tool life than a ramp, simply because it generally would result in better chip clearance, which could result in less re-cutting of chips. Maybe your flood coolant solves that, maybe not.
     
    JimDawson likes this.
  9. Metal

    Metal United States Active Member Active Member

    Likes Received:
    72
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    when you are ramping you are also cutting with more of the tool so you can go a little faster.
    fusion 360 also has a "profile ramp" which cuts roughly the shape of the final pocket's shape as part of the ramp which I use since it is less finicky about setting the ramp diameter correctly.
     
    JimDawson likes this.
  10. Boswell

    Boswell United States Hobby Machinist since 2010 H-M Supporter-Premium

    Likes Received:
    83
    Trophy Points:
    28
    City:
    Cedar Park
    State:
    Texas

    -Return to Top-

    When I was using CAMBAM it also would ramp on the profile shape external or internal I used this more than Sprial. But when I switched to BobCad the RAMP entry just seems to go in a straight line although there might be more config options I have not figured out yet.
     

Share This Page