Help with 5 Axis head/head post

[belformsam]

Help with 5 Axis head/head post, we are currently developing a 5 axis cnc machine for milling foam , we use mastercam x9 and have the multiaxis  option, the 5 axis post wont work with our machine as i think its a table/head, can i just edit the 5 axis post and machine definition that came with it , to suit our needs? or is there a 5 axis head/head post available for download? 

[Colin Gilchrist]

You only need to edit the Post file. The 5X post does not read the setup from the Machine Definition, only the post.

[belformsam]

ok, any help on modifying the post? how do i define the rotational axis b/c on the head? Also im not totally new to post processor writing/editing, just no experience with 5 axis post. 

[Colin Gilchrist]

Here are some basic settings to get you started:

 

mtype  :  2

 

------- rotaxis1 and rotdir1 set the "primary" axis. For a C-Axis (rotates about machine Z), you want 'vecx' and 'vecy' in the definition ------

rotaxis1$  =  vecy

rotdir1$  = vecx

 

 

-------- rotaxis2 and rotdir2 set the "secondary" axis. For a Gantry, the 'rotaxis2' setting is always 'vecz'. The rotdir2 can be either 'vecx' or 'vecy' depending on A/B (rotate on X or Y) --------

 

rotaxis2$ =  vecz

rotdir2$ = vecx

 

Now that you have the basic settings, you can fill in the other "Gantry" variables:

#Tool length, typically for head/head machine, both set to zero disables
#Applied to the tool length, RA applies this along the tool
drluseclr    : 0     #Use Drill Clearance Plane at start/end - 
                     #Read from toolpath parameters
use_tlength  : 0     #Use tool length, read from tool overall length 
                     #0=Use 'toollength' var, 1=Mastercam OAL, 2=Prompt
toollength   : 0     #Tool length if not read from overall length
shift_z_pvt  : 0     #Shift Z by tool length, head/head program to pivot (Z axis only)
                     #0=Pivot, 1=Pivot-Z, 2=Tool Tip Programming (without zero length)
                     #Option 2, So we can still take advantage of brk_mv_head feature
add_tl_to_lim : 0    #Add tool length after intersecting limit, always
                     #on if limit from stock
use_g45      : 1     #Use G45 offset with right angle head (RA)
g45_of_add   : 30    #Add this number to tool length no. for G45 offset number

You should enable 'use_tlength'. This variable "shifts" the XYZ coordinates from the Tool Tip, to the Pivot Point of the machine. Depending on the value (0, 1, or 2), Mastercam handles the tool length offset in different ways.

 

A setting of '0' uses the "toollength" variable (just below 'use_tlength'). A setting of '1' takes the Overall Length from the Tool Definition (must edit each tool to include the Gauge Length from pivot point to tool tip). A setting of '2'  will "prompt" the user for the tool length of each tool, during the posting process.

 

The post is built to assume that you "know" the pivot length of each tool. This will require measuring this value, and always keeping your tool lengths set to a "known" value, or it will require you to measure the tool lengths of every tool, then "repost" the NC code, using these "measured" gauge lengths.

 

After those basic settings are good, then you can set the Rotary Limits:

#Rotary axis travel limits, always in terms of normal angle output
#Set the absolute angles for axis travel on primary
pri_limlo$   : -9999
pri_limhi$   : 9999
#Set intermediate angle, in limits, for post to reposition machine
pri_intlo$   : -9999
pri_inthi$   : 9999

#Set the absolute angles for axis travel on secondary
sec_limlo$   : -30
sec_limhi$   : 120
#Set intermediate angle, in limits, for post to reposition machine
sec_intlo$   : -30
sec_inthi$   : 120

The "primary" setting is the C-Axis, and the "secondary" is the "tilt" axis. If your "primary" axis is "continuous" (allowed to "wind-up"), then +-9999 gives you 27.775 "revolutions" before the head will make an "unwind" move.

 

If your head is not "unlimited", you'll probably have limits like +-360, or 0-360, or +-200. Just enter the "high" limit as positive, and the "low" limit as a negative number.

[belformsam]

OK, thank you Colin, for the info and fast reply, i will play with these settings as you have described and hopefully it ll get us there. Do you know of any manual to help with this?

[belformsam]

ok, so i edited everything, now how do i install or use that post? when i have tried it the whole pst. file shows up in code editor, but no g code, what am i doing wrong?

[crazy^millman]

All 5 Axis post have a .psb file that has the nuts and bolts of them. Have you renamed the .pst file? Have you moved the .pst file and didn't move the .psb file? They go hand and hand if you rename one you must rename the other exactly the same name. They both must reside in the same folder. This is part of the MP.DLL smoke and mirror things I talk about. Nothing in a .pst tells the .psb to look for it and vice verse, yet the MP.DLL has logic written into it to sort this out.

[belformsam]

thanks that helped, i just copied the 5 axis psb file and renamed it as you said, now its posting gcode ! although the axis coordinates dont make sense, the numbers are too large, it shows min z travel in code editor at 50" and max at 12" ,my part is only 8" deep, same for all other axis, any ideas?

[belformsam]

i think i just stumbled on a 5 axis router post head/head, in the router post file folder, and it seems sort of setup and its not posting any crazy numbers in the code editor, i just changed the control definition for the generic 5 axis table/head machine definition, to use the 5 axis router post, bad idea? good idea? anyone else know anything about this?

[crazy^millman]

i think i just stumbled on a 5 axis router post head/head, in the router post file folder, and it seems sort of setup and its not posting any crazy numbers in the code editor, i just changed the control definition for the generic 5 axis table/head machine definition, to use the 5 axis router post, bad idea? good idea? anyone else know anything about this?

 

They are about the same post. Difference is the router posts have Aggregate Head stuff built in where as the Mill Post don't.

[belformsam]

ya it is the same post, just all the variables pertaining to a head/head setup were done, and im sure there are other differences about the router post i dont understand,  now hopefully it wont need too much tweaking to get it right for our machine.

[belformsam]

ok, so when i post a tool path mastercam prompts me to enter a tool length, is that the actual tool length? or the length from tool tip to center of rotating B axis? 

[crazy^millman]

ok, so when i post a tool path mastercam prompts me to enter a tool length, is that the actual tool length? or the length from tool tip to center of rotating B axis? 

 

There is a question in the post to make this question come up or not. Really comes down to he machine and how it figures out tool length, Newer machines will figure out the tool length and apply the difference from the actual to the pivot distance. Old machines you had to know the gauge length from Pivot to get good code to run the machine. If your machine does all the heavy lifting for you then you don't need to know anything and you program it like a 3 Axis machine. If you do then you can decide to use the OAL from the tool definition automatically and make sure you have that correct when defining the tools or you can keep a spread sheet of all your tools and their gauge lengths.

 

You have been at this for 3 days a post is cheaper than the amount of time you have wasted sorting all of this out.

[belformsam]

Ya, i wish my 3 days was worth $3500, cause thats what a custom post cost as per their quote. also i have spent a total of an hour maybe over the three days, why do you write posts?

[crazy^millman]

Ya, i wish my 3 days was worth $3500, cause thats what a custom post cost as per their quote. also i have spent a total of an hour maybe over the three days, why do you write posts?

 

Nope we buy them.

 

If your machine has been running 24/7 in those 3 days and the post has not been an issue then good, but many times people will spend weeks trying to get a post working. Every hour the machine is not making chips is 2 hours of lost production. 3 x 24 is 72 hours, but a total loss of 144 hours. If shop rate was just $50/hr then that is $7,200 of lost money. I am the crazy person around here so I will just mind my own business and wish you best of luck. I hope you get it all figured out and going with no wasted time on the machine what so ever.

[belformsam]

Hi everyone, so far we have the machine working as a 3 axis and it works well, now the problem is the b/c head, it seems to move along the shape properly but everything is skewed off about 90 deg on the c axis and a few degrees on the b axis, any ideas?