Absolute value VS. Incremental

[haroldm]

Hey guys.

I was wondering, and i suppose this is a rookie question, but what exactly do these two values mean? For example, i am surfacing a small dome part, and i was forced to use a parallel tool-path (dont ask) . So when the tool gets real deep, the machine slows down on the downward feed as it jumps over the hump., and that is what i am trying to change. Any suggestions would be appriciated, thanks.

[3R!< W3NG3R]

This sounds like a control thing to me. Are you filtering the toolpath?

[P_Scott]

haroldm,

 

Asolute values in the parameters are always in reference to the Origin (X0 Y0 Z0). Incremental in the operation parameters is related to the location of the selected geometry for the operation. These should not be confused with a G91 output in the code. Many new programmers are leary of using the Incremental because they associate that term with the G91 output. This term should read something like "From Geometry" or "From Chain".

 

For example, if you chain a contour on a 3-D wireframe that's at a -0.5" depth, Absolute value would have to be filled out to (-0.5) in the field. Selecting the same chain and using Incremental, set the value to (0.0) to get the toolpath to machine to the same depth of the chain. The output will still produce the proper depth (-0.5") but if the geometry is ever moved, the Incremental depth is associated to the chain and the depth value would not need to be changed before regenerating the operation. Also many contours could be done with the same tool in the same operation even if they are at differing depths.

HTH

 

P.S. This unfortunately has little or nothing to do with what you describe is happening at the machine.

[haroldm]

Thanks guys..i cant use the filter option because our xxxxor does not accept it. I was just trying to make the parallel cut go faster without having to resort to another type of tool path. Thanks.

[Thad]

quote:

---

i cant use the filter option because our xxxxor does not accept it.

---

How does the machine know that you filtered it? I can see if the machine doesn't like arcs in planes other than XY, but other than that, it's all G code. Set your filter to arcs in the XY plane only and see if that works.

 

Also, it sounds like maybe you're drip feeding your program and there is data starvation, thus the slow down.

 

Thad

[John Summers]

If you're using a bullnose cutter, it will 'flip' around when you get to the top of a dome (the surface normal points to tool center, and it changes direction abruptly at the top of the dome). If you did a spiral pocket from the center, you wouldn't see a 'bounce'.

[TonyNanni@BNB]

not sure exactly what you are talking about but sometimes if a tool path is making a lot of herky jerky motions try adjusting the gap setting, this will keep the tool down and a smoother tool path.

[Thee Rickster ™]

Maybe the path needs to be de-bugged, should it

not just cut smoother anyways, by 'default'.

[haroldm]

How about this guys..my material is 3.1 thick, i have set the feed plane to 3.2. Is there a way i can

get the tool to rapid down other than change the Feed number? I am getting a real slow downward feed and i was thinking maybe incremental vs absolute might be my problem? Thanks for the help.

[Guest]

Have you tried changing your feed plane to .1 incremental. That should get it to rapid down to .100 above the point where it will feed down the last .1

[haroldm]

Thanks John, I try that right now.

[Kannon]

switch your plunge rate in your tool parameters.

 

I will ask..

why do you only want to use surface parallel?

[haroldm]

haha..the boss wants it that way, i just follow orders. His business, his plan. Iwill also change the plunge rate, thanks for the help guys!

[tonyc]

"Have you tried changing your feed plane to .1 incremental. That should get it to rapid down to .100 above the point where it will feed down the last .1"--- johns words And thats what I would do.But do what the boss man says he pays

the bills

[Müřlıń®]

haroldm, do not change the plunge rate unless you are plunging too fast when you enter the stock on a plunge move.

 

On the para's page.

 

Set clearance to an absolute value.

Set retract to an absolute value.

 

Set feed plane to an INC value.

 

This will rapid down to feed plane instead of using the plunge rate.

 

Saving time...