Spiraled down cut


Results 1 to 10 of 10

Thread: Spiraled down cut

  1. #1
    Member shmity's Avatar
    Join Date
    Oct 2022
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Spiraled down cut

    Hi Folks,

    Im wondering if what im trying to do is possible in enroute. We bore quite a few holes(25mm diameter to 80mm diameter) in various materials (mdf, compact laminate, corian) and Id like to do this in a spiraled down cut in one pass rather than multiple thin passes with tool lifts. I've seen the function in Aspire but cant find anything similar in Enroute. Can anyone shed some light?


    Thanks

    Similar Threads:


  2. #2
    Member
    Join Date
    Nov 2013
    Posts
    4280
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Hi,
    I do the same thing in Fusion. I deselect the usual LeadIn/LeadOut and select Ramp instead. Does EnRoute have similar?

    Craig



  3. #3
    Member shmity's Avatar
    Join Date
    Oct 2022
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Thanks Craig. Not that I can find. The best I have been able to produce is a lead in/lead out at the radius of the cut, minus tool diameter that takes 90 degrees to spiral down and up. Which almost does the job and is adequate for MDF in 18mm and less but for solidsurfaces and thicker MDF I need it to spiral down at a much shallower rate.

    Edit: This is using Enroute 6.



  4. #4
    Member
    Join Date
    Nov 2013
    Posts
    4280
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Hi,
    shame, I find the Ramp lead-in quite useful. I often bore holes in fibreglass PCB, of many diameters. I find it useful to circularly interpolate those holes with a 1.5mm endmill
    rather than having dozens of different drills on hand. Ramping into the hole saves the shock loading on the endmill.

    The ramp feature allows me to chose the ramp angle and speed, either or both can be used to optimise the lead-in.

    Craig



  5. #5

    Default Re: Spiraled down cut

    Wow the time you're going to save....

    In Router Offset > Cut Definition

    Apply the settings as you would then goto Entry/Exit Parameters

    Under Entry
    Choose LINE
    Length: apply as long as you want, longer it is the longer the ramp
    Keep ANGLE at 0, change from default 10 to 0, otherwise it will come in at whatever angle is there
    3D Line to be Checked
    Lift @ 0

    Exit can be optional

    I just dont get what the Combination is. Probably dont have a need for it
    as Im going fine w/o it so far.

    See attached jpg

    Attached Thumbnails Attached Thumbnails Spiraled down cut-stew-jpg  


  6. #6
    Member shmity's Avatar
    Join Date
    Oct 2022
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Quote Originally Posted by Picktool View Post
    Wow the time you're going to save....

    In Router Offset > Cut Definition

    Apply the settings as you would then goto Entry/Exit Parameters

    Under Entry
    Choose LINE
    Length: apply as long as you want, longer it is the longer the ramp
    Keep ANGLE at 0, change from default 10 to 0, otherwise it will come in at whatever angle is there
    3D Line to be Checked
    Lift @ 0

    Exit can be optional

    I just dont get what the Combination is. Probably dont have a need for it
    as Im going fine w/o it so far.

    See attached jpg



    Thanks Picktool! Here I am thinking round hole, round entry. Just did a quick simulation and thats perfect!



  7. #7
    Member
    Join Date
    Nov 2013
    Posts
    4280
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Hi,
    I guess Fusion is similar, if the toolpath is circular then the ramp down is circular, if its a linear or modestly curved toolpath, then the ramp is linear or modestly curved also.
    Does EnRoute have a ramp down speed?. For instance the defined speeds in Fusion are g1 cutting speed, lead-in/lead-out speed, ramp speed and plunge speed.

    Craig



  8. #8
    Member shmity's Avatar
    Join Date
    Oct 2022
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Spiraled down cut

    Quote Originally Posted by joeavaerage View Post
    Hi,
    I guess Fusion is similar, if the toolpath is circular then the ramp down is circular, if its a linear or modestly curved toolpath, then the ramp is linear or modestly curved also.
    Does EnRoute have a ramp down speed?. For instance the defined speeds in Fusion are g1 cutting speed, lead-in/lead-out speed, ramp speed and plunge speed.

    Craig
    Unfortunately no, you can set the main cut feed rate, final cut feed rate and plunge speeds, but it looks like they are consistent across the tool path. But using picktools strategy, the longer the lead in the more loops in the spiral downcut the path takes, effectively slowing the plunge speed anyway.



  9. #9

    Default Re: Spiraled down cut

    Quote Originally Posted by shmity View Post
    Unfortunately no, you can set the main cut feed rate, final cut feed rate and plunge speeds, but it looks like they are consistent across the tool path. But using picktools strategy, the longer the lead in the more loops in the spiral downcut the path takes, effectively slowing the plunge speed anyway.
    You can also speed up the Z plunge and/or lengthen the Length to take lighter passes. Knowing the perimeter distance helps to to give an idea for small cuts. Same would work for Open Offset Contours as well. Since you're at it, save as a cut Strategy for frequent use. You'll need it because it gets tedious constantly applying it & sometimes forgetting.



  10. #10
    Member shmity's Avatar
    Join Date
    Oct 2022
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Picktool View Post
    You can also speed up the Z plunge and/or lengthen the Length to take lighter passes. Knowing the perimeter distance helps to to give an idea for small cuts. Same would work for Open Offset Contours as well. Since you're at it, save as a cut Strategy for frequent use. You'll need it because it gets tedious constantly applying it & sometimes forgetting.
    I've just finished creating strategies for all my common hole sizes for all our materials for exactly that reason.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Spiraled down cut

Spiraled down cut