Haimer Tool Offset and Z Height Problem - Page 2


Page 2 of 2 FirstFirst 12
Results 21 to 31 of 31

Thread: Haimer Tool Offset and Z Height Problem

  1. #21
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Ray explains the most efficient method. In the example I show above the bottom, front back and sides in first picture were the most critical surfaces of the entire part and they are all milled and finished. I always try to do as many critical sides as I can in the first cam offset. In this case I machined 5 precision surfaces from one offset and let the top of part be the wild surface and mill it to height and as parallel to the other 5 surfaces as possible in the previous setup. Then you have a decent 6 sided precision part to work on other sides with if required.

    Add a note it also helps to use decent feeds and speeds and be careful with small diameter tool overhang. Was chasing a problem last week. I didnt have same overhang set in hsm advisor and at the holder on the machine. Had I entered that value correct in hsm it would have warned me your not going to be happy with results due to tool deflection.



  2. #22
    Registered mnicholas77's Avatar
    Join Date
    Aug 2015
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    I appreciate all the input guys. I think we can all agree there are several ways to establish WCS and work holding setups, and as a stranger it helps to not assume anything to eliminate possible causes. I'm not new to machining and holding tolerances, but something is off here. The only subject thus far that has had a steady stream is setting up WCS in the CAM software. I mentioned earlier that I think my issue is the relationship between my Haimer offset and my WCS, which lends itself to how I'm setting up my parts in CAD/CAM and then executing. I think I'll try only using model WCS instead of stock and see where that gets me...right after I eliminate my tool height offset gauge.



  3. #23
    Member
    Join Date
    Oct 2010
    Location
    USA
    Posts
    670
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Try running it as Ray stated. I switched to this method and cut out nearly 99% of my height issues.

    I run the Hamier down to where my (machined edge) of my part will sit and zero the DRO out. This is the same location as what I have in Fusion 360 (I measure my part thickness after the facing operation and this is what I use for stock thickness in Fusion 360). Now, this is for the second operation..... When I'm facing or decking off the part on the first operation I sometimes will use the stock top just to make it easier and to allow for variations in stock thickness.

    Hope you get it dialed in. Nothing like chasing zeros + 10 to make ya go mad.

    Later,
    Awall

    Awall - The Body Armor Dude
    CoolCNCStuff_ on Instagram - CoolCNCStuff.com


  4. #24
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    I have both the Haimer and the ET offset gauge, and they do work. I actually touch off the Z more often with the ET than the Haimer, though I use the Haimer for initial setup.

    Something you can try is to put in your cutter tool (fly cutter?), set the ET on top of the work, touch off on the ET, enter 4.0000 for Z, and then do your cut. I do this often in case the tool has pulled out some and it keeps me to a though or less.

    Bob



  5. #25
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Ray also mentions he uses mostly g54 as his offset for a given part position. This is a great method and much simpler to setup in all cam system software on the market. The only difference is you have a G-code file for each side / position. It also allows easy post code edit to position the part where you want and any offset number. Also that frees up g55-g59 to use on different sides of the same part. Then you can line up the material in fixtures across the table and run the same file over and over just putting raw stock in fixture at left and remove complete finished parts off the right side. Steve mentions this in his posts. Always wanted to use this method because most of my 1100 table goes un-used

    Using a consistent ucs located at the bottom of material works very well and or with sprutcam its no problem using any fixed position on the vise, fixture, pin or some other magic point in space . Only time Rays method has bit me was about 0.125 oversize stock combined with high feeds and speeds with a marginally tight PDB oops leads to pullout and or material pull out and the big red button I run 5-6 parts watching material fly before I had a problem.

    Anyway Sorry I can't help more. Without a Hamier probe or a similar electronic device. I would not get anything done. I have a rack of tts height guages, edge finders 2 of each type and style all to find ucs positions. I try to keep extra Hamier probes in stock for the vary reason to avoid having to use them. Still they are required to pick up thin material edges or mini pallet screw down parts and hole centers.



  6. #26
    Registered mnicholas77's Avatar
    Join Date
    Aug 2015
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    Maybe I'm misunderstanding something. I use G54 already for any one particular part position, i.e. Set G54 At top of stock with the part .020" below stock surface and then machine down to top of part. Then OP2 gets a new G54 located at a feature of the part to pick up the part again on part bottom once flipped for decking and other bottom side features. I usually use carvesmart jaws with talon grip like feature built in for OP1 and then place part on parallels for OP2. I reference top of parallels for Z zero, then travel up the part thickness and re zero.

    Are you saying to keep my OP2 WCS zero point on the bottom of the part instead of raising it up the part thickness and resetting zero to part thickness? I'll give that a try but with instruments capable of reading down to tenths, why should it matter? If that's enough to create such wild part thickness variations, then there's a problem bigger than just where I choose to stick my WCS.

    Quote Originally Posted by mountaindew View Post
    Ray also mentions he uses mostly g54 as his offset for a given part position. This is a great method and much simpler to setup in all cam system software on the market. The only difference is you have a G-code file for each side / position. It also allows easy post code edit to position the part where you want and any offset number. Also that frees up g55-g59 to use on different sides of the same part. Then you can line up the material in fixtures across the table and run the same file over and over just putting raw stock in fixture at left and remove complete finished parts off the right side. Steve mentions this in his posts. Always wanted to use this method because most of my 1100 table goes un-used

    Using a consistent ucs located at the bottom of material works very well and or with sprutcam its no problem using any fixed position on the vise, fixture, pin or some other magic point in space . Only time Rays method has bit me was about 0.125 oversize stock combined with high feeds and speeds with a marginally tight PDB oops leads to pullout and or material pull out and the big red button I run 5-6 parts watching material fly before I had a problem.

    Anyway Sorry I can't help more. Without a Hamier probe or a similar electronic device. I would not get anything done. I have a rack of tts height guages, edge finders 2 of each type and style all to find ucs positions. I try to keep extra Hamier probes in stock for the vary reason to avoid having to use them. Still they are required to pick up thin material edges or mini pallet screw down parts and hole centers.




  7. #27
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Well If I understand this right your trying to use the machine dro / hamier probe with your cam program and machine a precision Z part height, using 2 different sides. While it can be done I have no such skills. Only time I do this I sneak up on it with a fly cutter or other tool. Measure and repeat and still I have marginal success or precision doing it that way. That said people do it all the time with manual machines with dro readouts.

    The example I show above uses the machine / cam ucs at top of part first side. Then bottom of part 2nd side and the cam does all the movements and math to the correct z height. I even mill past total part depth on sides on first side. Then when I flip the part and cut precision z height it has no bur and very clean cut to final height. I even play with tool paths here to provide a cool looking finish. The example above does not need that may passes. I like the concentric rectangle tool pattern that is left on surface.

    As mentioned above using this method I get parts precise enough in height its hard to measure them with my tools. In other word they all measure the same depending on temperature.



  8. #28
    Member
    Join Date
    Feb 2006
    Location
    USA
    Posts
    7063
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Quote Originally Posted by mountaindew View Post
    Ray also mentions he uses mostly g54 as his offset for a given part position. This is a great method and much simpler to setup in all cam system software on the market. The only difference is you have a G-code file for each side / position.
    Not so. I have a single g-code file, no matter how many fixtures/setups the part requires, and whether I use only G54, or several different fixtures (G54-G59). Every CAM I've ever used has allowed me to do this in a single g-code file. In particular, HSMXpress/HSMWorks/FusionCAM makes it truly trivial.

    Regards,
    Ray L.



  9. #29
    Member
    Join Date
    Aug 2009
    Location
    United States
    Posts
    294
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Quote Originally Posted by mnicholas77 View Post

    Are you saying to keep my OP2 WCS zero point on the bottom of the part instead of raising it up the part thickness and resetting zero to part thickness?
    I assumed that's what you were already doing...measure once and keeping the Z zero there. Have you checked your Z for lost motion? If you are setting the Z once, then moving up and resetting again, lost motion in the Z could be your .003" - .0035" problem.



  10. #30
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    Quote Originally Posted by SCzEngrgGroup View Post
    Reducing the number of fixture offsets is one way to minimize errors, and most parts, even when machined on all sides, can be made using a single fixture offset.

    Regards,
    Ray L.
    Quote Originally Posted by SCzEngrgGroup View Post
    Not so. I have a single g-code file, no matter how many fixtures/setups the part requires, and whether I use only G54, or several different fixtures (G54-G59). Every CAM I've ever used has allowed me to do this in a single g-code file. In particular, HSMXpress/HSMWorks/FusionCAM makes it truly trivial.

    Regards,
    Ray L.
    Understood, using one offset to machine a 4 sided part in my opinion would not be any less error proof then using 4 offsets. Only difference is in cam setup and my software would not deal with this well unless I split that program up and then combined into one file before running on machine. The simulation I rely on to keep me from breaking precision tools is all I have for us non pro cnc users and it works best as shown above for me anyway.



  11. #31
    Member
    Join Date
    Jun 2005
    Location
    USA
    Posts
    653
    Downloads
    0
    Uploads
    0

    Default Re: Haimer Tool Offset and Z Height Problem

    It's probably not this, but I got tripped up for a while when the probe tip on my Haimer loosened up a few turns.

    How are you setting tool lengths again?



Page 2 of 2 FirstFirst 12

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

Haimer Tool Offset and Z Height Problem

Haimer Tool Offset and Z Height Problem