5 axis post help... IT feedrates broken????

[gcode]

I've placed a zip2go named "finishing" in the

MCX2_Files folder in the ftp site.

Its a simple 5X swarf path for a new machine post

I'm working on.

 

The post is outputting good numbers, but I'm having a problem with inverse time.

 

I have the post set to tooltip inverse feed rates

and pivot point goce output.

If I change the OAL in the tool definiton,

the gcode changes. The numbers are correct,

but no matter what I do, the IT feedrate

does not change.

 

A gage lenght of 5 or 50 makes no difference.

 

This post started life as the

GENERIC HAAS VF-TR_SERIES 5X MILL that comes with

X2_MR2.

 

Sinces its a trunion machine IT feeds would not change with tool length.

 

IMO something invloved with the "mtype" variable

is locked down inside the psb.

 

If some of the 5X wizards (or someone from CNC) around here could look at it, I'd appreciate it.

[john316]

.

 

I haven't looked at that post yet but it sounds like your post is set-up to use the Mcam overall length for the code output. It's seperate from the feed control. You'll find it here:

 

#Tool length, typically for head/head machine, both set to zero disables

#Applied to the tool length, RA applies this along the tool

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

 

Having it set to 1 will use your Mcam overall length. Set it to zero to program to tooltip.

 

This one is from our gantry. It uses G43.1 with the pivot distance in the post and machine perameters.

 

use_tlength : 0 #Use tool length, read from tool overall length

#0=Use 'toollength' var, 1=Mastercam OAL, 2=Prompt

toollength : 9.8425 #Tool length if not read from overall length

 

 

HTH

 

BTW, did you get a chance to try that G53 yet or is that machine still taking a dump?

 

.

[gcode]

Kevin,

it makes no difference what those settings are..

If I change the OAL on the tool def page, the gcode will change the proper amount

the IT feed stays the same.. no matter what

I just tried the G53 H0 this morning..

It looks like its going to work

[john316]

.

 

If, when you say tool definition, you mean in the tool parameters in the Tool Manager, somewhere you have a setting that's taking the tool length from the tool def. Is there any other place besides the post to set that?

 

.

[Nils N]

gcode, don't know if this will help or not, I'm not a post guy, but this is what my post has on tool length;

 

 

#Nutating machine (mtype 3-5) describe the plane that the nutated axis

#lays in, this is the plane perpendicular to the primary axis and

#secondary axis

nut_ang_pri$ : -45 #Nutating head secondary axis angle from machine Z positive

 

#Tool length, typically for head/head machine, both set to zero disables

#Applied to the tool length, RA applies this along the tool

use_tlength : 1 #Use tool length, read from tool overall length #TF was 2

#0=Use 'toollength' var, 1=Mastercam OAL, 2=Prompt

toollength : 7.115 #Tool length if not read from overall length

shift_z_pvt : 1 #Shift Z by tool length, head/head program to pivot (Z axis only) #TF was 1 back to 1 10/27/05NN

#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 : 0 #Use G45 offset with right angle head (RA)

g45_of_add : 30 #Add this number to tool length no. for G45 offset number

[john316]

.

 

Hey G, I just downloaded your file and your post has a value of "1" for the "use_tlength" setting. Using that value takes the tool length from your tool def. in Mcam. With the G43.4 you are using you need to set that to "0" and put the pivot distance from your machine in the "toollength" setting on the next line down. Your machine has the pivot distance entered as a parameter and will use that along with the tool length offset to calculate it's final position.

 

.

[gcode]

John,

the gcode is right... I'm building parts with it.

The inverse time feed rate is not.

It stays the same whether the OAL tool length

is 0, 5.00", 50.00" or a million.

 

If I set the post to tool tip and run with g43.4

I get exactly the same feedrates as I do if I post pivot point and a 100" long tool. The inverse time feedrate never changes.

[john316]

.

 

Okay, I see what you're saying now. You're trying to get your feed right not your position. The feed won't change with tool tip because there's nothing to control the fanning ratio. Change your feed control to

#2 - tip to pivot on tool length

or

#3 - min-max on flute length to pivot on tool length

 

and see if that makes a difference. If you're using the tool length from Mcam option #3 will probably get you closer.

 

I tried your file with option #3 and it only affected the lead-in and lead-out. How close are the feeds your getting right now and what do you want different?

 

.

[gcode]

quote:

---

How close are the feeds your getting right now and what do you want different?

---

Not even close.. and ... I want them to work

 

If I post from the pivot point, the gcode is good but the feedrates are way too fast.

 

If I post tooltip, run g43.4 and let the machine

handle the feedrates we're getting by but we're cutting aluminum. When we start cutting steel we'll be in trouble.

 

I think something is broken in Machine Def.

I've got everything set right in there but

IT never changes.

 

I'm going to build a fresh V9 post and see what the feedrates are.

The old V9 pivot point posts Bruce and I built for the SNK gantries worked perfectly.

[john316]

.

 

Your programmed feedrate is 30ipm which make the inverse come out starting at F253.4 on your first line with inverse feed.

 

I changed the programmed feed in the Toolpath Manager to 5ipm and the first inverse feed came out to F48.1

 

Remember that is inverse time and not ipm. Is the F48.1 inverse closer to what you're looking for? It's about 20% of the original feed.

 

.

[gcode]

a bump in the hopes someone from CNC will look at this...

 

and an embarrassingly dumb question.

 

should inverse time feed rates change when the

gage length of a tool changes??... or is this something the machine controls from the pivot point...

[john316]

.

 

That is something the post builder would have to tell you because they know how they built the logic. But, you can see that changing the gauge length doesn't change your posted feedrate. One clue, watch the feedrate output at the control and compare it to the programmed feedrate. You might see a difference between the programmed feed and actual feed. That would tell me that the machine is calculating it's feed based on the programmed feed and the pivot distance+gauge length.

 

.

[Bruce Caulley]

Changing the gauge length shouldn't change the inverse feed. The machine handles that.

 

Bruce

[gcode]

quote:

---

Changing the gauge length shouldn't change the inverse feed

---

Thanks.. I was starting to think that was the case. I've got a couple of old prven posts

where the IT feedrate was changing, but

I think it was because the resoltion of the toolpath changes with the change length..

ie.. the feddrate wasn't changing, the distance

between each point changes therefore the F number

is different, but the results on the machine are the same.