[RayJ2395]

Pardon my ignorance about anything on here but I am new too all of this.

I recently acquired a well used '99 Haas VF4 in an attempt to learn CNC machining. Hopefully getting proficient enough to get a brand new machine down the line.

This is my first time designing the setups and making the program on Fusion, and I am attempting to do all this from youtube videos. I would really like to find a CNC course at a local college /trade school here in South FL, but I haven't found any yet.


Anyway to my current issue i need to overcome...

I believe I have set up the machine correctly. G54 is correct and all the tool offsets (3) have been set.

Prior to starting the program I make sure XY and Z are in their home position. Z all the way up and the x and y far left and forward.

I start the program the X & Y position themselves correctly but from what i can see in the code the program is asking Z to go up .55 and it throws a Z over travel alarm.

(Note: when All Axis are home X&& read 0 where as Z reads, 4.5...) ?

N10 G90 G17
N15 G20
N20 G53 G0 Z0.

(Adaptive5)
N25 T4 M6
N30 S5000 M3
N35 G54
N40 G17 G90
N45 M8
N50 G0 X-0.0245 Y-6.2871
N55 G43 Z0.55 H4 <---Right here is where the Z over travel error
N60 T2
N65 G0 Z0.15
N70 Z-0.25
N75 G1 Z-0.275 F20.


I would appreciate any help (things to look for, videos to watch, etc), as I said I am completely new and all of this still sounds like a different language to me but I'm working it out.
Thanks
Ray

[jxdxwx]

You are very close to cutting chips. Approach with caution. Would advise taking vises and fixtures off the table and practice with no tools until you fully understand the offsets.

You said G54 and all tool offsets are correct. Your explanation sounds like you zeroed your work coordinates at your machines home coordinates with no offsets referencing the location of your workpiece in relation to your machine coordinates.

A hint may also be on tool #4 length offset. Should be a large negative number. (example measurement from the tip of your tool to a part in your vise, it may read: -15.000 or so etc.)

Post a snapshot of your offsets pages that show your work coordinates and tool offsets.

[bostosh]

How about a different approach?
What part do you want to make first?
I recommend an
"other than gcode learning experience"
First, i can send you thousands of lines of proven Gcode
And a cad file of your table with parts material and gcode too list.
This starts with an overall concept and then work into Gcodes.

And your machining experience please.

(we generated Gcode on punched teletype tape from computers in 1970) I had to learn the BCD codes of the frickin punched tape) it is soooo easy now 10,000 lines with no errors

[RayJ2395]

jxdxwx: That is correct the tool offsets are a large Negative value, -18.xxx (attached picture, tool 1 is not included in the operations)
Also it appears the Z when home reset, as now when the machine is in its start up home position all read 0.
Good call on removing the fixture. I'll do that now.

Sorry for the delayed response, back in front of the machine again.

Thanks for your help!

[RayJ2395]

How about a different approach?
What part do you want to make first?
I recommend an
"other than gcode learning experience"
First, i can send you thousands of lines of proven Gcode
And a cad file of your table with parts material and gcode too list.
This starts with an overall concept and then work into Gcodes.

And your machining experience please.

(we generated Gcode on punched teletype tape from computers in 1970) I had to learn the BCD codes of the frickin punched tape) it is soooo easy now 10,000 lines with no errors

Absolutely I would love some good gcode lines so I can run them on the machine with no tools or fixture to get my bearings. I'm all ears on any learning materials.

Thanks!

[Superman]

jxdxwx: That is correct the tool offsets are a large Negative value, -18.xxx (attached picture, tool 1 is not included in the operations)
Also it appears the Z when home reset, as now when the machine is in its start up home position all read 0.
Good call on removing the fixture. I'll do that now.

Sorry for the delayed response, back in front of the machine again.

Thanks for your help!

You are missing pic of the work offset page...
But...
Going by your pics, the values that go into G54 would be negative... as that is transferring the datum from machine position to be on the workpiece.

Now.... depending on how you are referencing the G54 Z position ( most use a reference tool, others use the spindle face ) the G43 says to "add" the length offset value to that reference point to move it to the tooltip.

What I don't understand is how you have 18" of tool length when the part Z is only 13.6" from your reference tool point

The value in tool length offset is the distance fron your reference position to the tool tip
Ie. if you use spindle nose as reference, 4" of holder body plus 1.5" of tool stick out should be offset value of 5.5"
If you use the spindle nose as your ref point, I think your offset values should be positive

Remember G43 adds the values, so -13.6 plus -18.25 wants to move -31.85"

That is why your Z wants to go up, up and away
it wants to bring the tooltip at -31.25 to the Z0.55 plane

[RayJ2395]

You are missing pic of the work offset page...
But...
Going by your pics, the values that go into G54 would be negative... as that is transferring the datum from machine position to be on the workpiece.

Now.... depending on how you are referencing the G54 Z position ( most use a reference tool, others use the spindle face ) the G43 says to "add" the length offset value to that reference point to move it to the tooltip.

What I don't understand is how you have 18" of tool length when the part Z is only 13.6" from your reference tool point

The value in tool length offset is the distance fron your reference position to the tool tip
Ie. if you use spindle nose as reference, 4" of holder body plus 1.5" of tool stick out should be offset value of 5.5"
If you use the spindle nose as your ref point, I think your offset values should be positive

Remember G43 adds the values, so -13.6 plus -18.25 wants to move -31.85"

That is why your Z wants to go up, up and away
it wants to bring the tooltip at -31.25 to the Z0.55 plane

Well, Success you your explanation made me see what I was doing wrong.

The G54 is/was negative but that main screen had it as a positive value... (picture attached of the G-54 now)

Ran the program without any fixture, test the height of Z and it was good to go.

Mounted the fixture and machined 3 edges of the aluminum block before I damaged my end mill. Due to me not putting the exact stock dimensions. I was off by .035 on one side and .025, that and no coolant (wanted to see better) led to the end mill break.

Loading up the coolant, tweaking the program and I should be able to run my program without anymore issues.

[Superman]

Well, Success you your explanation made me see what I was doing wrong.

The G54 is/was negative but that main screen had it as a positive value... (picture attached of the G-54 now)

Ran the program without any fixture, test the height of Z and it was good to go.

Mounted the fixture and machined 3 edges of the aluminum block before I damaged my end mill. Due to me not putting the exact stock dimensions. I was off by .035 on one side and .025, that and no coolant (wanted to see better) led to the end mill break.

Loading up the coolant, tweaking the program and I should be able to run my program without anymore issues.

The G54 Z value should be negative... because that is where it is in 3D space in respect to machine's home position & the reference tool point
Your tool length offsets (+,-, actual length) are what needs to be sorted out.... normally the build length and it is positive... If the reference point is the spindle nose.
Offset lengths is the distance you want to have that reference point translated

[countryguy]

Not sure it matters but I was just chatting w/ a guy today on a 98 and he needed the pre-NGC post processor for Fusion. Not the NGC one. Just a thought.

[bostosh]

Can someone clarify the acronym NGC Thanks!

[countryguy]

Can someone clarify the acronym NGC Thanks!

pretty sure it's Next Generation Controller. and for the PP https://cam.autodesk.com/hsmposts ( if HSMWorks for CAM).

[bostosh]

Thank You for clarifying the acronym update to a dated programmer.
The first controller generation i ran parts on had vacuum tubes.
Punched paper tape converted to real-time run magnetic tape.
Programmed with pencils and APT.