Inverse feedrates 5axis

[David Colin]

Hi all,

 

I am not really comfortable with 5 axis toolpathes and i am wondering about inverse feedrates for my postprocessor. Every formula I read don't use rotary axis to calculate tool movement (and time). Is this really the way to go? I'm thinking about an impeller blade finishing toolpath for example. It looks like, only using XYZ points to make calculation, sometimes involve rotary motions too fast...

 

Any idea?

[Dan@home]

3 X 360 DEG per min= F1080. That is not that fast (3 revolutions or full turns per min), If it is cutting 15" in Dia, then yes it is fast.

Cutting 3" Dia then that it would be alot slower.

[Rocketmachinist]

I would look up my manufacturer information on my mill. It will tell you max feed rates in every axis along with max spindle speed. Then you can go into the machine definitions manager and put those values in. For example, your machine only has a 10,000 rpm spindle and you write a program where the spindle speed is 12,000 then it will give you an error message and not let you do that. The same thing happens with the additional axis. If the feed is too high then it will error out also.

[David Colin]

My problem isn't that i exceed machine specifications but that I'd like to get a constant tool load and smooth tool motion.

[Matt Sumner]

Inverse time is a good method to use for multi-axis work because it is consistent whether using rotary or linear or both together. Basically the feed is the inverse of the time it takes for the move to occur. That means all the axis involved in the move will end up at the final position at once at the end of that time period. The actual F command is expressed as the inverse of that time, normally in minutes. So 0.5 seconds becomes 0.00833 minutes and therefore F is equal to 120. If you're using a post that has a good calculation for inverse time then it should work great and will take into account feeds changing due to diameter.

 

However any feed method will work well as long as the calculation is done correctly in the post and the machine control accepts it. If you're getting problems you might need to get your post looked at .

 

Hope that helps.

[Josh T™]

I personally use inverse feeds for all of my rotary machines. I find that the feed rates and tool transitions are much smoother and consistant.

 

What machine are you trying this on?

[dolphin1]

quote:

---

smooth tool motion

---

usually you need to use a command to set for multi-axis machining with smooth motion. with the Variaxis i use its G05 P2 on and P0 for off.

hth

[Matt Sumner]

Smooth motion and constant tool load are more affected by the programmed path. Lots of points will create very smooth motion as long as your controller can handle all the information and still maintain the desired feed rate. Often either the control gets bogged down with all the code or the max feed rates are too low to keep up with the programmed motion. Depends on the machine.

 

It's usually better to use a feed rate that's lower than you would like in order to let the machine keep up smoothly.

[David Colin]

Machine is a Mazak integrex 200 Matrix 6 months old. Post-processor, well, I'm looking into it as I need to do a 5-axis job soon. Inverse time should be ok with my machine control (G93 G-code) and i am convinced this is the way to go.

 

But here is a good point from Matt :

"If you're using a post that has a good calculation for inverse time then it should work great and will take into account feeds changing due to diameter."

 

I try to optimize these calculations because I read almost everywhere formula below to calculate length of the toolpath (which is needed to calculate inverse feed):

Length = sqr((Prv_x$-x$)^2+(Prv_y$-y$)^2+(Prv_z$-z$)^2)

 

But what's happening if during the toolpath, tooltip position almost doesn't change but tool direction does (so only 4th and 5th rotary axis) a lot? Well rotary axises are gonna move very fast as time calculated will be near zero.

 

So I think this kind of calculation is ok if you're machining with tooltip only (bull nose) but for, for example swarf machining it's not reliable... So if anyone have an idea?

[Matt Sumner]

The mazak should have an option for 3-D cutter compensation. When using that function it may compensate in some cases for the effect you are talking about.

 

What needs to happen to elimante the issue is to calculate feed based on the distance travelled by the contact point of the cutter to the work piece. This is not too difficult in 2-D operations. For example normal cutter compensation G41 & G42 will do it on some machines. It and can even be done in some 3-D ops when using a ballnose cutter as I mentioned above. However when you try to calculate the effective feed rate on something like a swarf operation it's impossible in some cases. Imagine a swarf op on the outer surface of a cone that comes to a point. At the bottom of the cone the feed is close to correct but on the pointed end it's infinately too slow.

 

I hope I didn't go too far off track there.