Pocket Toolpaths Still Run Through a Boss, After All These Years

[Leon82]

I had a pocket do that years ago. It was good and when I changed the step over from 50 to 55% it went thru the center boss

[Jobnt]

17 minutes ago, JoshC said:

i was gonna say is no one going to suggest a modern toolpath, pocket is sooooo outdated.... nothing wrong with doing things the old way, but if improvements can be made why not do it, dynamics only scary at first, then it just becomes the norm 

Not gonna lie, I don't use the modern toolpaths much because I haven't been trained on them and I get really bad results most of the time, but once I get over this hump I will try to get familiar with them. 

It just cracks me up that Mastercam has had this issue for decades and STILL can't won't fix it. 

[byte]

57 minutes ago, Jobnt said:

Not gonna lie, I don't use the modern toolpaths much because I haven't been trained on them and I get really bad results most of the time, but once I get over this hump I will try to get familiar with them. 

It just cracks me up that Mastercam has had this issue for decades and STILL can't won't fix it. 

One of the things pocket does well that Mastercam doesn't is nested pockets,

here i selected 2 solid surfaces as drive, one using pocket, & one using Area Mill

The pocket operation machines the selected regions as expected

Selecting the same surfaces in Area Mill with Automatic Regions yields this result

This is Mastercam 2024 PC2 I think, I haven't installed the new Beta, but I do not think this has been fixed, you can create one operation per surface, but that can become impractical if there are hundreds

Another feature we need in 2d hmm is keep tool down for outside pockets, I have requests for both of these open 

[Jobnt]

Interesting. One thing I love about Mastercam is there are a dozen ways to do just about everything. One thing I don't like about Mastercam is there are a dozen ways to do just about everything. 

Once I figure out the best strategies for the parts we do this will get easier. 

In the mean time, expect some dumb questions the next few months while I get back in the groove. 

[cncappsjames]

I took Mastercam at Mt. San Antonio College... in 1992 or 1993 IIRC. V3.1 was the 1st semester for 2D... they moved us to V4 the 2nd Semester. 

MCTV FTW!

[cncappsjames]

When I have an issue with a 2D toolpath the 1st thing I do is change the strategy (one way vs. Zig-Zag vs. Spiral, or morph spiral vs constant overlap, etc...), next I change the steopver percentage, then I'll change chaining order. Or after that there's still no joy, I'll change toolpath type. One of those ALWAYS works. 100% of the time. 

[Jobnt]

I use a different order but yes, same basic steps and have always gotten it to work. Sometimes it just takes a lot longer to find a solution.

/ranton
There's a lot about MC that just bugs me, like the backplot window always changing size and the #*@&ing POS active reports viewer always opening full screen. My monitor is 3 feet wide and almost 2 feet tall. 

I. Don't. Want. ANY. Window. To. Open. Full. Screen.

Ever. 
/rantoff

[Aaron Eberhard]

I believe with all of 2d toolpaths, the intention is that you select the point first, then the toolpath chains.  I'm surprised it worked at all with the point afterwards.

Quote

Use entry/exit point

Uses the last point chained before the toolpath chain as the start point for entry moves, and as the exit point for exit moves.

But like others, this regens fine in any versions I have installed (22-24), so at least this particular issue was fixed 3 or 4 years ago.

[Colin Gilchrist]

For what it's worth, I was able to get decent results with regular "Pocket", but only if I turned off "spiral inside to outside".

The algorithm doesn't like nested chains, with 'spiral inside to outside' enabled.

One of the great things about 2D Dynamic paths > they support "different types of chains". So you can have "cut geometry", "avoidance geometry", and "air geometry". In addition, there is a set of radio buttons that allows you to change strategy from "Stay inside" to "From outside". With "From outside" selected, the path will naturally attempt to simply plunge outside the cut area, without using an "entry method" of ramp or helix.

By using the Air Chains, you can tell the system if there are "pockets" inside the geometry that have already been roughed out, or if there are exterior edges of the shape being machined, that are in "open air".

 

Pocket Start Point Fail.mcam

[Jobnt]

42 minutes ago, Colin Gilchrist said:

The algorithm doesn't like nested chains, with 'spiral inside to outside' enabled.

 

That's my go-to path. Sounds like a very slight change in my work habits will fix this ongoing issue. 

I've spent a few hours playing with dynamic paths and now that I understand a little better what all the regions are for and how to chain them I think I'll be spending a lot more time with them vs the old school stuff. 

Thanks much for the help everyone, including Ron.  

[Aaron Eberhard]

3 minutes ago, Jobnt said:

That's my go-to path. Sounds like a very slight change in my work habits will fix this ongoing issue. 

I've spent a few hours playing with dynamic paths and now that I understand a little better what all the regions are for and how to chain them I think I'll be spending a lot more time with them vs the old school stuff. 

Thanks much for the help everyone, including Ron.  

Good luck on your journey into Dynamic paths.  If you haven't seen it yet, make sure you hit the "preview Chains" button in the chaining dialog.  It will show you exactly what you've told the algorithm to cut, so you can immediately know whether you're going to get what you want out it before even entering parameters.

[Jobnt]

There's a lot more to it than there used to be for sure, and WAY more than the "other" software" ever thought of having. 

[cruzila]

Quote

Interesting. One thing I love about Mastercam is there are a dozen ways to do just about everything. One thing I don't like about Mastercam is there are a dozen ways to do just about everything. 

This could become my new tagline!!!

[Aaron Eberhard]

Oh, yeah, a few other thing to know going into Dynamic paths, in no particular order:

* Use a good High Speed calculator.  I use HSM Advisor, but the Harvey Tool/Helical calculator app is awesome as well.

* Use the full flute length, unless it's excessive.  For example, if you have a 3" deep pocket w/ a 1/2" endmill, go at least 1" deep per pass if you have the flute length.

These settings:

will control how successful you are in your cut.  The minimum toolpath radius is "what is the smallest radius this toolpath can create" and it will be machine dependent.  if you're cutting mild steel with a good spindle, you may find yourself running at 500-600 IPM, but your machine can only keep up @ 500 IPM in a radius of .100", anything smaller than that and it starts to slow down.  Either make the radius smaller or the whole path slower to keep an even chip load.

The microlift & backfeed rates are the most often overlooked time savings in it, you can often shave off 30-40% of your cycle time by setting that right.  The microlift is how much it pulls off the surface to travel across it between cuts so it doesn't drag the tool in the surface or chips, and the back feed rate is how fast it does it.  On a reasonably modern machine, a .003-.005" lift and whatever the max feed rate of your machine is should go in there. 

 

[Jobnt]

18 minutes ago, Aaron Eberhard said:

Oh, yeah, a few other thing to know going into Dynamic paths, in no particular order:

* Use a good High Speed calculator.  I use HSM Advisor, but the Harvey Tool/Helical calculator app is awesome as well.

* Use the full flute length, unless it's excessive.  For example, if you have a 3" deep pocket w/ a 1/2" endmill, go at least 1" deep per pass if you have the flute length.

These settings:

will control how successful you are in your cut.  The minimum toolpath radius is "what is the smallest radius this toolpath can create" and it will be machine dependent.  if you're cutting mild steel with a good spindle, you may find yourself running at 500-600 IPM, but your machine can only keep up @ 500 IPM in a radius of .100", anything smaller than that and it starts to slow down.  Either make the radius smaller or the whole path slower to keep an even chip load.

The microlift & backfeed rates are the most often overlooked time savings in it, you can often shave off 30-40% of your cycle time by setting that right.  The microlift is how much it pulls off the surface to travel across it between cuts so it doesn't drag the tool in the surface or chips, and the back feed rate is how fast it does it.  On a reasonably modern machine, a .003-.005" lift and whatever the max feed rate of your machine is should go in there. 

 

Great info, thanks. 

I'm very familiar with Volumill (GibbScam) and most of the settings you mentioned are there. My biggest hurdle I think is setting the chaining correctly. Once I figure that out I'll prolly quit asking so many stupid questions.

 

[JoshC]

20 minutes ago, Jobnt said:

Great info, thanks. 

I'm very familiar with Volumill (GibbScam) and most of the settings you mentioned are there. My biggest hurdle I think is setting the chaining correctly. Once I figure that out I'll prolly quit asking so many stupid questions.

 

caminstructor Mike who makes incredible mastercam training videos has a free youtube channel where he posts some of their free offerings and he has an entire video series found here if your interested, 

, and on top of that their actual caminstructor courses avalable for purchase are very good training courses, so if you like what he shows there you may want to check out their caminstructor website as well. 

 

Alternatively i have been really liking Titan of cnc's video courses, and many of their offerings are also free resources, here is a link to some of their vids which may be helpful, i think these vids utilize more of the 3d optirough instead of 2d dynamic, but both are great paths to learn and utilize. https://academy.titansofcnc.com/series/titan-building-blocks-mill-in-mastercam-cam

[gcode]

1 hour ago, Jobnt said:

Great info, thanks. 

I'm very familiar with Volumill (GibbScam) and most of the settings you mentioned are there. My biggest hurdle I think is setting the chaining correctly. Once I figure that out I'll prolly quit asking so many stupid questions.

 

Chaining Dynamic milling toolpaths is counterintuitive, at least it is to me.

The machining region will normally be your stock.

Avoidance regions are normally your finished part (ie you want to avoid cutting it) 

Air regions are exactly what they say they are.

Once you get the hang of it, you can do some pretty amazing stuff by manipulating the machining and avoidance region chains

[Jobnt]

19 minutes ago, gcode said:

Chaining Dynamic milling toolpaths is counterintuitive, at least it is to me.

The machining region will normally be your stock.

Avoidance regions are normally your finished part (ie you want to avoid cutting it) 

Air regions are exactly what they say they are.

Once you get the hang of it, you can do some pretty amazing stuff by manipulating the machining and avoidance region chains

It kind of is to me, too. GibbScam uses Volumill for dynamic milling. The biggest difference I see is that you have to create air-walls as a geometry type then Volumill sees it and drives the toolpath accordingly. Most of the other chaining is very similar. 

I've spent most of the day upgrading some toolpaths on a travel fixture to use dynamic and have gotten a lot better with it.

[Sumac Andy]

I unchecked the 'spiral inside to outside' and worked fine for me?

 

Andy.

[Jobnt]

36 minutes ago, Sumac Andy said:

I unchecked the 'spiral inside to outside' and worked fine for me?

 

Andy.

 

 

Not my preferred strategy.  

[Colin Gilchrist]

For using the Dynamic Paths, here are some typical good starting values.

As Aaron mentioned, try to utilize a much flute as possible, but I try and stay between 2:1 and 3:1, Depth-to-Diameter ratio. As you get above 3:1, you'll need to reduce your Stepover accordingly.

For Aluminum, I typically use between 20-40% Radial Engagement (Stepover), depending on cutter length. For 2:1, or under, go with 40% to keep the material removal rates up. I think 30% is a good "default" stepover value for aluminum. That said, I've successfully done an outside shape with 4:1 ratio (2" deep with a .500 diameter tool), but dropped my stepover to 15%.

Typical Stepovers, based on material, at 2:1 Ratio:

Aluminum

15-40%, default of 30%

Steel

10-20%, default of 15%

Stainless Steel

5-15%, default of 8%

HSRA (Inconel, Waspalloy, etc.)

2-5%, default of 2.5%

Titanium

2-6%, default of 4%

 

I try and keep my "minimum corner radius" value at double my stepover value, or more. If you're trying to get the tool into tight areas, like a slot between features, you can drop this value down as low as 3% (minimum input value I think is 2.5%).

For "Pockets", you do not need any Avoidance Geometry. You only need Machining Geometry, set to "Stay Inside". (You can use "Avoidance" for internal bosses however.)

As G-Code mentioned: you do need Machining Geometry for Stock, and Avoidance Geometry for the part contour, when roughing an external shape from outside.