Horizontal Drill

[Jaz]

I will try to get the details first try.

4 axis horizontal machine. Machine def and control files based off standard 4-axis HMC that come w/ MCam.

I drive a curve 5-axis toolpath, that works fine. (I did have to translate everything to be parallel to the system top plane to make it work )WCS looking down at top of pallet, TPlane front, rotary axis = Z. Generates fine, backplots good, posts good code.

 

I drive a drill 5-axis toolpath w/ points and lines. NO GOOD.

1) front TPlane, rotary axis = Z; backplots drilling sideways, posts bad.

2) top TPlane, rotary axis = Z; backplots good, posts bad.

3) front TPlane, rotary axis = Y; backplots good, posts good, BUT when I open the saved file it replaces my machine w/ default and will not let me replace my machine until I change rotary axis = Z

 

I have been able to get the same effects with the 4-axis HMC that comes w/ MCam.

 

Can someone tell me what I am doing wrong? Why would the TPlane and rotary axis settings work for curve 5-axis and not drill 5-axis?

 

Also would like to be able to leave my parts out in aircraft coodinates rather than move them.

 

Thanks

ps,

I cannot load a sample file, my internet access is limited.

[K2csq7]

I program my HMC's as VMC's...

 

The help of your reseller is in order. They will be able to (they should) take the time to get to know the details of your situation and provide you with a "correct" process.

 

Are some of the holes not parallel to your Z axis? I ask because I am wondering why your using multiaxis drilling toolpaths instead of the 2d drill path.

If you cannot post a file, screenshots will help.

 

 

2) top TPlane, rotary axis = Z; backplots good, posts bad.

3) front TPlane, rotary axis = Y; backplots good, posts good, BUT when I open the saved file it replaces my machine w/ default and will not let me replace my machine until I change rotary axis = Z

 

 

For #2, have you checked to see if you can change the axis of rotation for your rotary inside your post?

For #3, That is the method I would think should work (your tombstone does rotate about Y). I have not seen a machine def get replaced like that....

[Jaz]

All my holes are parallel to the spindle.

I'm drilling 5-axis because I have 96 holes into a cylindrical surface and I'm lazy.

[Richard Thomas - Mastercam UK]

Wow. I thought "there must be a logical reason for this" but no, I can't work it out either. Does yours spit out B180, B360 type calls regardless on the expected B axis angle?

 

Now I have to admit that when I can't get something to work, I tend to try a bit too hard to get the results I want. So, I did manage to get toolpath that seems to do what I'd expect in terms of B axis numbers. But you won't like it...

 

Set your Planes to Top and start a standard (2d) drill operation. Pick the points that you want to drill (at the end of your lines I presume). In the parameters, go to the Planes page. Keep the WCS to Top, set the Tool Plane to Front and keep the Construction Plane at Top! (so the tool is in HMC orientation, but Mcam is "looking" at the points from the top down.

 

Now, go to the Rotary Axis Control page. Set the Rotation Type to "Rotary axis positioning", go to the option below and rotate about the Z axis (that's the Z axis of the Cplane I believe although technically speaking I could be mistaken). Apart from Axis Substition, I rarly use these other options I have to admit.

 

The Backplot looks right on my file (as long as the Linking Params are set sensibly), and I get Y and B axis moves that I think would run on a HMC.

HMC ROTARY.MCX-6

T.txt

[gcode]

I'm not going to go into the details of why this is happening because I really don't understand it myself

but.. the HBM machine defs think " you can't get there from here" and won't do it.

 

there is a fix however

 

go into your machine def and add "Four Outlet Right Angle Aggregate" head to your Tool Spindle.

this will have no effect on posted code or machine def operation, but will trick it into

properly running 5axis toolpaths on a 4 axis horizontal mill.

 

the other option is to set up a VMC post (Top WCS / Top TP=B0) for your HBM

 

you'll have to play around with the rotation axis in the toolpaths, but it does work when you get everything

set right.

 

I started doing this in X5.. I can't say if it works in earlier versions

 

see the attached screen shot

[Guest CNC Apps Guy 1]

Now I have to admit that when I can't get something to work, I tend to try a bit too hard to get the results I want. So, I did manage to get toolpath that seems to do what I'd expect in terms of B axis numbers. But you won't like it...

ROFL and yep. I hear you.

 

 

I'm not going to go into the details of why this is happening because I really don't understand it myself but.. the HBM machine defs think " you can't get there from here" and won't do it.

I hate when that hapens.

 

...there is a fix however...

There usually is thankfully.

[Ron Branch @ 5th Axis]

Tom how in the world did you find a hack like that?

[gcode]

Tom how in the world did you find a hack like that?

 

 

I added an aggregate head to a machine def trying to do some right angle head work ( and failed)

months later I tried a 5X toolpath and it worked..

when I went to post it for a different machine my 5X toolpaths blew up ...

so I went searching for the differences in the machine defs

 

now all my HBM machine defs have a phony 4axis aggregate head

[Guest CNC Apps Guy 1]

I REALLY LOATHE MACHINE DEFS!!!

[Ron Branch @ 5th Axis]

LOL that is some funny stuff right there.

[?Mark]

I REALLY LOATHE MACHINE DEFS!!!

 

+1

LOL, they screwed up more thing that they ever helped with...

[gcode]

they for sure have not lived up to the advanced billing we got in early X days

[crazy^millman]

they for sure have not lived up to the advanced billing we got in early X days

:whistle: :whistle: :whistle: :whistle:

[Guest CNC Apps Guy 1]

they for sure have not lived up to the advanced billing we got in early X days

 

 

True dat. I wish they would scrap it all together and just have switches in the post for axis information and orientation. The Control Def is a little better but still, thing were MUCH better when that stuff was handled by switches in the post.

[Jaz]

OK. I've got 2 work arounds to try. I'll get back with you.

[K2csq7]

True dat. I wish they would scrap it all together and just have switches in the post for axis information and orientation. The Control Def is a little better but still, thing were MUCH better when that stuff was handled by switches in the post.

 

+100

[Greg Williams]

+1000

[Jaz]

gcode - you are the champ . 'course we all knew that.

Added an aggregate head to the spindle, left all the settings, etc. at default. Everything now does what I expect.

 

Rich Thomas - I was not able to get you method to work for me. I can get good code but files doe not reload correctly.

 

Thank you everybody.

[gcode]

glad I could help