Reverse and Swap axis help!

[WildBill9000]

We have a vertical / horizontal mill (two heads, one vertical on a slide, one horizontal). It is programmed as a vertical mill. The problem is when in horizontal mode everything is backwards and upside down. I need to reverse X and swap Z with Y. I have been playing with the machine component manager and it appears to do nothing at all. If I draw the part in the plane I want (Back Gview) I still get z moves for clearance and y for cutting, with no reversal of x. The same goes for a top WCS and back t/c planes.

[Craig-B]

You should try to useing the front view for horizontal milling B0. Front.

[K2csq7]

I think your going to have to use 2 different machine defs with 2 different wcs's... not sure how else you would get the reversal of x...is all the machining done with the control in g17?

[WildBill9000]

Machining is done in G17-19. What does the machine component manager do then? Most horizontal mills have replaceable heads, I would think mastercam would have a feature like this somewhere without having to edit the post.

[K2csq7]

Most horizontal mills have replaceable heads,

I would't say "most".

I think you need to contact your reseller, it sounds to me like your going to need aggregate capabilities or something at the very least.

[WildBill9000]

Alrighty, I can edit the post to get "Z" output instead of "Y" and vice-versa (also swapped K with J). Is there a way to mirror moves over X in the post? I can use transform toolpath to mirror over x and then post it, but it would be much slicker to draw it normally and have it post mirrored.

[Jimmy Wakeford from Barefoot CNC]

You can set the variable scalex$ to -1 to reverse/mirror the x

[WildBill9000]

I am not seeing that variable in the post, do I need to add it?

[Jimmy Wakeford from Barefoot CNC]

yes, you can just type it in:

scalex$ = -1

[WildBill9000]

I can stick that anywhere in the top of the post right? Nothing is happening. I have it here ->

 

# Common User-defined Variable Initializations (not switches!)

# --------------------------------------------------------------------------

xia : 0 #Formatted absolute value for X incremental calculations

yia : 0 #Formatted absolute value for Y incremental calculations

zia : 0 #Formatted absolute value for Z incremental calculations

 

bld : 0 #Block delete active

result : 0 #Return value for functions

sav_spc : 0 #Save spaces

sav_gcode : 0 #Gcode saved

sav_absinc : 0 #Absolute/Incremental Saved Value

sav_coolant : 0 #Coolant saved

sav_frc_wcs : 0 #Force work offset flag saved

toolchng : 1 #On a toolchange flag

spdir2 : 1 #Copy for safe spindle direction calculation

scalex$=-1

[Jimmy Wakeford from Barefoot CNC]

Okay, I'd tried it and its broke.

Not recomended, but this will flip X

pfxout          #Force X axis output
xabs = xabs * -1
xinc = xinc * -1
     if absinc$ = zero, *xabs, !xinc
     else, *xinc, !xabs

pxout           #X output
xabs = xabs * -1
xinc = xinc * -1
     if absinc$ = zero, xabs, !xinc
     else, xinc, !xabs

 

I changed those two post blocks to get it to work, also need to swap G02 and G03.

 

I say not recomended cause I don't know what post your using. You can try it and see if it breaks anything on your post.

[Jim Evans from CNC Software]

scalex, scaley, scalez are not broke or at least shouldn't be. Their use is tied to the fastmode switch (has been since v8 I believe - scale variables are ignored when fastmode is on.). We also do NOT recommend using the Scale X,Y,Z variables because of their inconsistent use inside of the MP executable. For wire it is typically ok to use them but I would still shy away from them.

 

Modifying the post depends on the post you are using and how you are programming in Mastercam and. You could easily setup your machine definition to handle both the VMC and HMC spindle using axis combination so that the post can be written to read the axis combo and make the necessary calculation adjustments based on what you program.

 

You should contact your reseller and get them to have a post guy look at it and quote the work. It will save you lots of time and headaches in the long run.

[Jimmy Wakeford from Barefoot CNC]

Jim, I tried scalex$ with fastmode 0 and nothing. I haven't used it in forever, but thought it still worked. I tested it with mpfan.pst. Also tried inverting the x axis in machdef under componet properties.

[WildBill9000]

Okay, I'd tried it and its broke.

Not recomended, but this will flip X

pfxout          #Force X axis output
xabs = xabs * -1
xinc = xinc * -1
     if absinc$ = zero, *xabs, !xinc
     else, *xinc, !xabs

pxout           #X output
xabs = xabs * -1
xinc = xinc * -1
     if absinc$ = zero, xabs, !xinc
     else, xinc, !xabs

 

I changed those two post blocks to get it to work, also need to swap G02 and G03.

 

I say not recomended cause I don't know what post your using. You can try it and see if it breaks anything on your post.

 

 

This works great! Thanks!

[master blaster]

I know this post is a little old but if someone could help it would be appreciated, I have a similar issue to the one mentioned above and have tried the mentioned fix and  it works great problem is the "I" value when cutting arcs also needs to be inverted. any suggestions on how to do this?

[jlw™]

Look and see if you have pfiout and piout and do the same.

[Colin Gilchrist]

What post processor are you using?

 

Try adding "iout = iout * -1", at the top of the 'pcirout' post block...

[master blaster]

using X5,

works great, thanks for the help