Feature Request Linear to ID/OD feed rate convertion

[David Colin]

Even if Mastercam HSM toolpaths expose radial engagement, it actually calculates engagement angle from it (and tool diameter) then maintain it (or as a not too exceed value). AFAIK all dynamic toolpaths engines work like that.

[Guest]

I don't think angle of engagement is superior to percentage of diameter. I think in it's current (and continuing development) state the differences between Volumill's strategies and Mastercam's Dynamic Path's are miniscule at best.

[jlw™]

Personally I think radial engagement matters way more than angle of engagement. I think angle of engagement doesn't really matter until you're greater than 50% such as inserted cutters plowing it where you want to engage thick to thin. Doing so will help with the lines the back of the cutter always leave when the cutter finnaly hits full tool pressure. I don't think endmills do this, at least I've never seen it myself. However, you can over engage radially no matter the angle.

 

I do like the line of sight changes in Dynamic and I can see changes in cycle time in several of my long run parts with feedmills.

 

to quote pegleg shorthorn: jm2cfwiw

[Sticky]

Engagement angle is a dynamic variable that changes with the profile being cut. Radial engagement is a static value. The two are not really comparable. I am not saying that radial engagement is pointless or anything of the sort, but it is a poor indication of cutting performance.

 

I'll try to create an obvious example.

 

Let's say we have a 40 taper spindle holding a 5 flute .375" diameter endmill, the gage length of the tool assembly is 12". We'll run the tool at 400sfm.

 

We have two cuts to make, both with a radial engagement of .02" The material is 4140 PH.

 

Mill a straight  line.

 

Interpolate a bore .5" diameter.

 

Which one is going provide a satisfactory finish and not chatter? Which one is going to howl and scrap your part? Even with proper feed correction for the bore, the engagement angle is going to be too high to get acceptable results. The issue is that the engagement angle is too great, regardless of the fact that the radial engagement is the same for both profiles.

[jlw™]

No offense sticky but thats a terrible example. You're comparing a straight linear cut to essentially a full medial bury. The dynamic or trumill paths both are engineered to prevent over engagement. The whole idea is to reduce engagement and keep it consistent. Other than corners that are 90° or less the human eye and ear wouldn't even be able to tell them apart.

 

Esprit had Profitmilling and I liked it but to be honest I'll take dynamic every day. The toolpaths yield EXTREMELY similar paths as does truemill and waveform but the dynamic paths are significantly easier/faster to set up.

[Sticky]

It's actually a great example, maybe a bit extreme, but it's clear you understand at least half the problem and can acknowledge that the bore example would provide unfavorable results. If we took the same example and applied it to a 1" bore you would still have poor results as the straight line cut has less than 20 degrees engagement angle and a 1" bore would have several times that.

 

The point was that radial engagement/stepover does not give an accurate indication to cutting performance, while engagement angle does.

[civiceg]

Using a 4th axis post, limited to 3 axis output, I had to disable the rot on x line under pmiscint$. Hopefully, I can get on a machine to do some testing this week. 

 

pmiscint$        #Capture the top level absinc for subprograms

      if sub_level$ <= zero, absinc$ = mi2$

      #Disable cutpos2 if not 4 axis, saves time

      #if rot_on_x = zero, cutpos2$ = m_one       <-- This line

[David Colin]

Mastercam HSM toolpaths are using engagement angle to generate paths.

 

There is an interesting post from ahaslam in this thread:

http://www.emastercam.com/board/topic/88622-2d-dynamic-question-x9/?hl=%2Bengagement+%2Bangle#entry1080474

[civiceg]

I think the complaint is that you can not limit or specify the engagement angle, as you can with the step over. 

[David Colin]

So yes cnc could easily improve Gui but it seems this is not what they do best

However knowing tool angle engagement (alpha):

Radial_depth_of_cut = tool_radius * (1-COS(alpha))

[Sticky]

I think the complaint is that you can not limit or specify the engagement angle, as you can with the step over. 

 

You got it.

[Matthew Hajicek - Singularity]

 

 

So yes cnc could easily improve Gui but it seems this is not what they do best

 

2nd.

 

One thing I think they could improve would be to calculate stepovers from the part out rather than from the stock extents in.  Doing the latter as it currently does often results in tall, thin ribbons which snag and chip flutes.

[Colin Gilchrist]

I'd like to see some modifications made to the way that outside sharp corners on the stock are machined. Currently the paths try to "round" the corners, and this has been a problem for many users, especially in hard materials. I think it really increases the angle of engagement during that move. I'm not sure what the best fix would be, but I was thinking that the path could sort of add an extra "loop" pass on these corners to reduce the material engagement.

 

I've often resorted to taking the corners of the block, and making several HSM paths to just clear away the corners. (Turn the corner into a "triangle" of material as the "stock", and put a boundary on the "part side" of the triangle to force the tool to only cut away the corner of the stock material.) Doing this adds extra work, but the results when running the "main path" are really sweet if there isn't that sharp corner on the material boundary.

 

In other news, I spent a whole bunch of time this past holiday weekend improving the code to slow down and speed up the internal/external arc feed adjustments. I need to do a little more testing, but I think that anyone who is interested will really like the results.

 

Here are some of the coming changes:

 

• Improved path and edge length calculations that don't just use the radius values, but take into account the actual length of the path, based on the sweep of each arc.
• Decelerated Arc Entry - I added some code to Circle Mill paths for the entry and exit moves. On the Entry Arc, the code will now calculate the ratio between the "next arc (adjusted feed value)", and the "current arc", and it will break the entry arc into line segments, each with a decreasing feed value. This has the effect of slowing the entry.
• Overrides for Lead In/Out (Contour) and Entry Line/Arc (Circle Mill), to use the programmed entry feed values, instead of the calculated values, if you enter values into the dialog box.
• Lead Out moves assume "programmed feed", and not "adjusted feed", in order to speed up the exit move (since the material is already cut away).
• I added some code for the Semi-Finish and Finish Feedrate Overrides for Circle Mill (specifically) to allow you to enter a Feed per Tooth value, instead of a Unit per Minute value. The logic will detect Feed values below .05, and will automatically assume these are FPT values, and calculate the proper Feed values, based on path vs. edge length.
• Circle Mill Semi-Finish and Finish Scallop Report - When using Semi-Finish and Finish passes with Circle Mill, the logic will attempt to calculate what the "advance per tooth" value is, based on the Edge Length of the arc being cut. This function will output a Comment Record before each finish pass arc, reporting the calculated APT value. (This is to help you discern what kind of finish you might be able to expect, from a given Speed/Feed combination being used.)

 

Maybe I should have rethought this whole donation thing? Lol, just kidding. I'm happy to contribute if people get some good value out of the code I've written. Who knows, maybe CNC Software will take some notice and incorporate some of these changes into the interface, so that these post modifications are no longer necessary. (But where is the fun in that?)

[MIL-TFP-41]

I started playing with doing this also. While nowhere near as refined as what you have, I was able to get a few things to work. One of the things I did a little different was 'a$$ume' that when climb milling a G3 would always be an internal arc and G2 would be an external arc. This way on a contour around a part it would compensate for both external and internal. Say a shape like the one attached. I don't have anywhere near the expertise...I couldn't get it to work properly on a lead in arc...so grabbing that idea from you.

 

Just some thoughts

 

[Brian Pallas]

Thanks for posting this Colin.  I had thought this was interesting when I first saw it, and put it in my mpmaster post I use for the horizontal machines today.  I like it. For some reason though, on the first depth cut of a toolpath I am not getting the adjusted feedrates on the arcs.  I am using post version  V16.00 P0 E1 W16.00 T1369940991 M16.00 I0 O1 of mpmaster.  Might anyone have an idea of why that would be, or what to look at?   

 

 

Edit : I just noticed that if the toolpath that is using the arc feedrate adjustment is not the first toolpath being posted, it works just fine.  The problem I have is showing up if the toolpath with the arc feedrate adjustment is the first toolpath being posted, and only on the first depth cut.

 

 

( 1/2 FLAT ENDMILL  TOOL - 1  DIA. OFF. - 1  LEN. - 1  DIA. - .5)
(COMPENSATION TYPE - WEAR COMP)
T1 ( 1/2 FLAT ENDMILL)
M01
M98 P8000
M06
M08
(MAX - Z6.)
(MIN - Z-1.05)
G00 G17 G90 G54
X.2 Y1. B0. S9500 M03
G43 H1 Z6.
Z.1
G94 G01 Z-.35 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0.
G01 Y0.
G03 X.25 I.25 J0.
G01 Y1.
Y1.03
G40 X.2
Y1.
Z-.7 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
Y1.
Z-1.05 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
G00 Z6.
G91 G30 Z0. M05
G91 G30 X0. Y0. M09
G0G28B0.
G90
M30
%

[Colin Gilchrist]

12 hours ago, Brian Pallas said:

Thanks for posting this Colin.  I had thought this was interesting when I first saw it, and put it in my mpmaster post I use for the horizontal machines today.  I like it. For some reason though, on the first depth cut of a toolpath I am not getting the adjusted feedrates on the arcs.  I am using post version  V16.00 P0 E1 W16.00 T1369940991 M16.00 I0 O1 of mpmaster.  Might anyone have an idea of why that would be, or what to look at?   

 

 

Edit : I just noticed that if the toolpath that is using the arc feedrate adjustment is not the first toolpath being posted, it works just fine.  The problem I have is showing up if the toolpath with the arc feedrate adjustment is the first toolpath being posted, and only on the first depth cut.

 

 

( 1/2 FLAT ENDMILL  TOOL - 1  DIA. OFF. - 1  LEN. - 1  DIA. - .5)
(COMPENSATION TYPE - WEAR COMP)
T1 ( 1/2 FLAT ENDMILL)
M01
M98 P8000
M06
M08
(MAX - Z6.)
(MIN - Z-1.05)
G00 G17 G90 G54
X.2 Y1. B0. S9500 M03
G43 H1 Z6.
Z.1
G94 G01 Z-.35 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0.
G01 Y0.
G03 X.25 I.25 J0.
G01 Y1.
Y1.03
G40 X.2
Y1.
Z-.7 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
Y1.
Z-1.05 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
G00 Z6.
G91 G30 Z0. M05
G91 G30 X0. Y0. M09
G0G28B0.
G90
M30
%

Not sure off hand, but something must be preventing the output. Have you tried running through the debugger? Set some Variable watches, and breakpoints, and you should be able to find it easily.

I do know the NCI formatting is the same for all motion. It is NCI G-Code 0, 1, 2, or 3, for 3X motion, and 11 for 5X motion.

[Colin Gilchrist]

13 hours ago, Brian Pallas said:

Thanks for posting this Colin.  I had thought this was interesting when I first saw it, and put it in my mpmaster post I use for the horizontal machines today.  I like it. For some reason though, on the first depth cut of a toolpath I am not getting the adjusted feedrates on the arcs.  I am using post version  V16.00 P0 E1 W16.00 T1369940991 M16.00 I0 O1 of mpmaster.  Might anyone have an idea of why that would be, or what to look at?   

 

 

Edit : I just noticed that if the toolpath that is using the arc feedrate adjustment is not the first toolpath being posted, it works just fine.  The problem I have is showing up if the toolpath with the arc feedrate adjustment is the first toolpath being posted, and only on the first depth cut.

 

 

( 1/2 FLAT ENDMILL  TOOL - 1  DIA. OFF. - 1  LEN. - 1  DIA. - .5)
(COMPENSATION TYPE - WEAR COMP)
T1 ( 1/2 FLAT ENDMILL)
M01
M98 P8000
M06
M08
(MAX - Z6.)
(MIN - Z-1.05)
G00 G17 G90 G54
X.2 Y1. B0. S9500 M03
G43 H1 Z6.
Z.1
G94 G01 Z-.35 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0.
G01 Y0.
G03 X.25 I.25 J0.
G01 Y1.
Y1.03
G40 X.2
Y1.
Z-.7 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
Y1.
Z-1.05 F250.
G41 D1 X.25 F100.
Y2.
G03 X-.25 I-.25 J0. F50.
G01 Y0. F100.
G03 X.25 I.25 J0. F50.
G01 Y1. F100.
Y1.03
G40 X.2
G00 Z6.
G91 G30 Z0. M05
G91 G30 X0. Y0. M09
G0G28B0.
G90
M30
%

 

The code uses both "feed <> back_feed", and the value of Misc Integer #10 as conditions. Also the value of 'cutpos2$'.

Only the HST operations (both 2D and 3D) would output the 'back_feed' value. So it is probably 'cutpos2$' being assigned different values. Your code doesn't look like it has helix moves, so my guess is 'cutpos2$' or maybe the value of 'mi10$' isn't set on the first pass?

[David Colin]

FYI, 2D contour filter has been improved in 2018 and it will adjust feeds with ID/OD.