5-Axis Gouging

[Colin Gilchrist]

Depending on the year/make/model of the Haas, the Maximum Inverse Time value can be as high as: 45000.00.

[Colin Gilchrist]

Reko,

 

Inverse Time is much different from normal Inch per Minute feedrate output. The value that is output in Inverse Time mode (G93) is actually the inverse of the amount of time it takes to complete that move. Its seems counter-intuitive, but the larger the value, the slower the move. The smaller the value is, the faster the move will be executed.

[Reko]

Reko,

 

Inverse Time is much different from normal Inch per Minute feedrate output. The value that is output in Inverse Time mode (G93) is actually the inverse of the amount of time it takes to complete that move. Its seems counter-intuitive, but the larger the value, the slower the move. The smaller the value is, the faster the move will be executed.

 

That makes me think our Haas is set up wrong.

 

When it was moving in those 4 corners that gouged... it was feeding at 999.99

 

Then, we changed it to F150. manually, and it slowed down and machined without gouging.

 

I always thought the inverse feedrate was based on time to complete the motion... because of the rotary motion.

[Guyinthedesert]

That makes me think our Haas is set up wrong.

 

When it was moving in those 4 corners that gouged... it was feeding at 999.99

 

Then, we changed it to F150. manually, and it slowed down and machined without gouging.

 

I always thought the inverse feedrate was based on time to complete the motion.

 

Are you in G93 or G94? Inverse time is the amount of time it takes to complete the move. F150. is way faster than F999.99

If you were trying to machine at 999.99 IPM, a gouge might be expected.

[Reko]

I'm in G93 and on the Haas I am using... F999. spins the rotary tables at top speed.

 

F150... is very slow.

[Reko]

Reko,

 

Inverse Time is much different from normal Inch per Minute feedrate output. The value that is output in Inverse Time mode (G93) is actually the inverse of the amount of time it takes to complete that move. Its seems counter-intuitive, but the larger the value, the slower the move. The smaller the value is, the faster the move will be executed.

 

Colin,

 

So, within the Haas control, is there a setting that could be reversed?

 

My program is output from Mastercam in the way that you describe... the 4 gouged areas on my part had F999.99 on the lines in that area, while the rest of the program seemed to hover around F400. to F600.

 

If the machine worked in the way you are saying it should, F999.99 would have slowed down and not gouged.

 

I am trying to contact Haas to get more answers on the machine side of things, but if anyone with Haas 5-axis experience can shed some light, I would appreciate it.

 

This is a new Haas machine and perhaps it is not set up properly.

 

Thanks!

[gcode]

try changing the F999 setting in your post to F9999

[Colin Gilchrist]

Hi Reko,

 

I took a look on Haas' website, and I gave you incorrect info before. The Feedrate in Inverse Time mode can be though of as "strokes per minute". To figure out how fast the move will occur, divide 60 by the feed value. This tells you the number of seconds the move should take to complete.

 

So for your numbers:

 

60 / F999. = .06006 seconds to complete

60 / F150 = .4 seconds to complete the move

 

So what you are seeing is correct. You'll need to adjust the Linear feedrate specified in your operation, until the value you input gives you the correct inverse value at the machine.

[Reko]

Ah, that makes more sense according to what is happening on the machine.

 

I wish there was a way to slow the toolpath down in specific area's, like where it makes large A or B axis swings... THAT is where the cutter overshoots and gouges the part.

 

@ gcode... I will have to wait until the next 5-axis job to experiment further as this job is complete.

 

I have been reading other posts here as well as other websites and it looks like the Haas could achieve up to 40,000 units of feed in inverse time, so I will have to look into that more, because the post I have caps the inverse feed at 999.

 

The way I got this part to come out good without gouging was to set the max to 150 but the rest of the toolpath was slooooowwwww.

 

I guess my goal is to understand how to max the feedrate in flatter area's... and slow the feed in steeper area's... which is where the A-axis trunnion tips and the B-axis platter spins quickly to maintain sync with the XYZ moves.

 

Slowing the A-axis and B-axis in steep area's is my goal... which right now, my post kicks out big numbers.

[Guyinthedesert]

What model rotary are you using?

[Colin Gilchrist]

It sounds like you need more tool axis vectors in the quick areas (more rotation on the rotaries) and less in the flat areas. You can usually achieve this by outputting a ton of tool vectors (make a really tight cut tolerance), and then using the Filter function to reduce the vectors based on the filter tolerance. I've still got your sample file, so I'll play around with the settings and send you a copy once I've made some adjustments...

 

Thanks,

 

Colin

[CJep]

What about using feed control zones in the utility section of the advanced multi-x toolpath, select the surfaces where you want the tool to slow down or speed up. You can also set an offset that allows you to slow it down before it hits the zone. Using the parallel to a curve would be the closest to the curve 5 and you could still use control lines for the TAC.

[Reko]

What model rotary are you using?

 

TR310

[Tyler Robertson]

It sounds like you need more tool axis vectors in the quick areas (more rotation on the rotaries) and less in the flat areas. You can usually achieve this by outputting a ton of tool vectors (make a really tight cut tolerance), and then using the Filter function to reduce the vectors based on the filter tolerance. I've still got your sample file, so I'll play around with the settings and send you a copy once I've made some adjustments...

 

Thanks,

 

Colin

 

tolerance + Angle step. I think 'Angle Step' should be renamed 'Angle Tolerance' because when you explain it to someone they inevitably say "So it's like an angle tolerance?"

[Reko]

It sounds like you need more tool axis vectors in the quick areas (more rotation on the rotaries) and less in the flat areas. You can usually achieve this by outputting a ton of tool vectors (make a really tight cut tolerance), and then using the Filter function to reduce the vectors based on the filter tolerance. I've still got your sample file, so I'll play around with the settings and send you a copy once I've made some adjustments...

 

Thanks,

 

Colin

 

I see what you are saying... it sounds like there are a lot of ways to accomplish what I am trying to get... I just need more experience forcing what I want to happen.

 

If you can get slower "F" rates in the 4 area's that the arrows point at, at the top of this post, I'd like to see how you accomplished that.

 

Thanks!

[Reko]

What about using feed control zones in the utility section of the advanced multi-x toolpath, select the surfaces where you want the tool to slow down or speed up. You can also set an offset that allows you to slow it down before it hits the zone. Using the parallel to a curve would be the closest to the curve 5 and you could still use control lines for the TAC.

 

Wow, that looks more powerful yet.

 

What blows my mind, is how the rotaries will take off out of sync from the XYZ moves.... that is what burned me here because I didn't realize that would happen.

 

Still, with the options within the 5-axis toolpaths, I can see now, there are ways to control that.

[CJep]

What blows my mind, is how the rotaries will take off out of sync from the XYZ moves.... that is what burned me here because I didn't realize that would happen.

 

Well, for the most part when doing 5 axis programming we are working with applied physics and dimensional calculus, we're using Mcam to run the higher math equations, by setting various parameters in the toolpath we are setting the formatting of the equation.

 

The condition your seeing the 5 axis moves sounds simiar to a condition that can happen when using high speed tpaths in a machine that is not considered a HS machine.

Acceleration & deceleration clearances, if the move is to small to make at the prescribed feedrate, ugliness ensues, usually just a bunch of feed limiter noise in the servos till you back off the feed. Now add in two more axis', rotation and time.

[rellim_63]

I've been trying to figure this problem out for a long time also. So, to fix the problem, the feed rate needs slowed down. Does this need slowed down in mastercam, because I have slowed down the federate before manually but it seems that it's in the code to do "loops" in these areas.

 

I am guessing these gauges the person is referring to is the "loops" that I'm getting?

[Reko]

Rellim,

 

I'm not certain what you mean by "loops." If you could post a picture, that would help.

 

My toolpath tried to follow the proper route, but it would overshoot and (seemingly) back up a bit to correct itself to stay on the toolpath. This happened in 4 area's of extreme A and B axis movement. THAT is where it gouged, or violated the surface, of the part.

 

The toolpath backplotted and verified perfect within Mastercam... but did not track properly at the machine.

 

Slowing the "F" rates solved my problem on this part... but I'm not certain what I did was the most efficient fix... because I just capped the whole part's "F" output at F150. which caused the whole toolpath to feed verrrry slooowwww.

 

A better solution would be to force slower F output only in area's of large A/B axis movement.

 

I am working on that.

[gcode]

Take the time to learn the advanced 5 axis toolpaths.

Buy the InHouse Advanced 5X tutorial and work your way through it.

There is enough power in that suite of tools to solve almost any 5 axis problem you might encounter

[crazy^millman]

Reko sorry, but kind of the nature of the beast you are programming. Like gcode said the advanced toolpaths have tones of capabilities. I would also think about a custom post. One that looks to the kinematics of the machine and then makes code not one that just makes code based off of formulas.

[Reko]

"Reko sorry, but kind of the nature of the beast you are programming."

 

Don't misunderstand... I'm loving this stuff... and I know I am just at the tip of the proverbial iceberg here, as well.

Also, I didn't know a better post was available for the Haas... I really thought these machines were so widely used, that the post would be tweaked as well as possible by now.

 

 

@gcode... I plan on that... I didn't know there was an advanced book available. Thanks.

[CJep]

Take the time to learn the advanced 5 axis toolpaths.

Buy the InHouse Advanced 5X tutorial and work your way through it.

There is enough power in that suite of tools to solve almost any 5 axis problem you might encounter

 

I would suggest the IHS Handbook Volume 3 as well, it breaks down the functions of each of the utilities in the multiaxis toolpaths with visual references.

[Colin Gilchrist]

Hey Tom,

 

Are you using the Adaptive Clearing with the Triangle Mesh toolpaths? That lets you create Dynamic style Toolpath motion with the Advanced Multi-axis Toolpaths. I've been generating some awesome paths with it lately. I then take the Adaptive Path, and use the 3X to 5X Toolpath to get the tool axis control I need. The end result is a full 5X path with Dynamic motion, and all the collision control you need. I especially love being able to set a Zig-Zag cut pattern with the Adaptive Clearing. With Zig-Zag, you can independently set the Climb engagement and the Conventional engagement as a percentage of the max step over. This means your tool never cuts air as it cleans out the corners of the material. I really like using 100% of the step over for climbing, and 35% for the conventional cuts. It lets me squeeze out a little quicker cycle time...

[crazy^millman]

Colin anything you can share? I would love to see in what ways you are getting it to work.