Pocketing toolpath - slivers and tear out

[Blackhawk]

I cut a large sign from 20lb Duna HDU. I used a .50" endmill at a .25 depth with 60% overlap to remove the background around the lettering. I used an offset strategy since it saved a considerable amount of machining time based on the estimation.

The problem with the toolpath that Aspire created is that it seems random and inefficient on where it starts cutting, then stops and then moves to another area for no apparent reason. This strategy causes puck marks or divots in the HDU. What happens is that the toolpath leaves these narrow slivers. Then when the cutter finally comes back to clean up the slivers, the narrow slivers start to tear away before they are cut. (See pic labeled "slivers") This tearing leaves the puck marks. (see pic labeled tearout).

What is really puzzling is my pic labeled "hole"? The toolpath sends the cutter to just make this one hole then pulls up and goes to another area instead of cleaning out the full area. There seems to be way too many unnecessary Z movements being created.

All of these pictures were taken while the machine was running.

Is a raster strategy the only improvement that I could have done? Is there any other setting in the toolpath creation that would help?

[adze_cnc]

Any step-over greter than the tool radius is going leave “slivers” to clean up later.

[Rcnewcomb]

with 60% overlap

I'm not quite sure what you mean by overlap. If your stepover is greater than 50% it will occasionally leave material. Try setting the stepover to 40%. (See image)

Regarding improving machine time, a ShopBot PRT Alpha running a 1/2" end mill in HDU should be able to cut in a single pass, so I would increase the pass depth setting on the end mill. Use ramping and specify a 2" ramp.

You can also create a toolpath for each portion of your design so that the portion is completely machined before moving on.

Also, raster vs. offset can change the strategy used and the machine time.

[Blackhawk]

Overlap = stepover. I did do this in a single pass. I understand that a smaller overlap would help with slivers. The run time is 4 hours at 60% stepover, dropping to 40% is going to add considerable time. Using a raster pattern was going to add an entire hour to the cutting time.

Like I say, I can understand some slivers, but I can't come up with any explanation to the toolpathing that you see in my last pic (labeled "hole"). I don't know any reason that it should cut two pockets in such a large area, then pull up and go to a completely different area 20" away. Once it starts in the middle of an area, I would like it to work from the inside/out until it cleans up the whole area.

My pocket area is within a border, the toolpath started out with 3 passes right up next to the border, then moved to the inside. This caused many of the slivers, like you see in the pic labeled "slivers". If it just started in the middle and worked it's way to the border, the very last sliver would be up against the border, so it would be basically non-existent.

[TReischl]

It may not seem logical to you, or there may be no "reason" that you can see but pocketing routines are all about logic. They are not just written willy nilly. I would hazard a guess that over the last 40 years or so tens of thousands of hours have been invested in refining them. Just so you know, software writers do not just sit down at their keyboards and say "Today I am going write a pocketing routine." We all do the same thing, we spend a lot of time researching various methods, algorithms, etc before we even write the first line of code. A pocketing routine is not a trivial exercise in programming.

Give you an example, you would like it to just start on the inside and work itself out to the boundary. Sounds simple, and with a simple rectangle or other basic shape it is simple. But what happens when there are islands, or reentries on that border? Quickly the simple becomes complex.

The slivers are not only caused by the software, in fact, it might be said that the software does not cause them at all. After all, the software drove the tool everywhere it needed to go to remove the material. How the tool interacted with the material is another matter. It would be nice if we could throw a tool in the chuck and every cut came out perfect. But there is a skill to cutting material, type of tool, carbide or hss, number of flutes, amount of helix, the list is almost endless. Tools do not come in all these wide varieties for no reason, it is because materials react differently to them.

Since this software has cut literally thousands of signs out of HDU over the years, if I were you, I would start looking at the techniques being used, things like the stepover amount, etc. I would also take a look at the tools I was using.

The hole you are annoyed by could well be caused by the amount of stepover you applied.

I can share something with you that annoys me to no end. People who want to hog out material all in one go, then complain about the finish and other issues. They should watch a few videos on machining, it is rare to see someone who does this stuff professionally not take a finish cut to achieve good results. Yea, I know, "that takes longer". It is what it is, a person can spend hours and hours being frustrated, blaming their tools, their machine, the software or they can get on with it and take a finish cut.

[Blackhawk]

TReishl - I apologize that I struck I nerve with you. This was not my intent. I was looking for advice on how to improve my toolpathing strategy and techniques as I asked in my original post. I joined this forum in 2008 and have been using Vectric software since before Aspire came out. I have used Aspire since the original version. If I came off as being critical of the software, I am again sorry. I try to learn and get better on every job that I do, which I hope everyone does in all things.


Can others please comment if they routinely run a finish pass when doing 1/4" deep pockets in HDU to clean up the bottom? If yes, how thick is the final layer that you remove for the finish pass? Do you increase feed rate for this final pass to shorten the cut time?

[Rcnewcomb]

The long run time and the "random" jumping may be indicators of excessive nodes.

I'd recommend reviewing your vectors to see if you can apply some smoothing, or if you can edit and remove some nodes.

You should also send your file to support@vectric.com to have them review it to see if they have suggestions for you, or if they have improvements that they need to make to their toolpath algorithms.

[chemstock]

Bits need to be sharp sharp sharp. synthetic material (not sure about HDU) use a glue that is very hard on bits. A dull bit will start to tear the material rather than cut it. If you have enough power on your spindle, increase the chip load, that may reduce the markings left on the material.

[TReischl]

TReishl - I apologize that I struck I nerve with you. This was not my intent. I was looking for advice on how to improve my toolpathing strategy and techniques as I asked in my original post. I joined this forum in 2008 and have been using Vectric software since before Aspire came out. I have used Aspire since the original version. If I came off as being critical of the software, I am again sorry. I try to learn and get better on every job that I do, which I hope everyone does in all things.


Can others please comment if they routinely run a finish pass when doing 1/4" deep pockets in HDU to clean up the bottom? If yes, how thick is the final layer that you remove for the finish pass? Do you increase feed rate for this final pass to shorten the cut time?

No need to apologize, no nerve was struck, and even if you had, still no need to apologize.

What I was trying to point out is that it is easy to get frustrated and then finger point. Doesn't solve the problem unless something is actually the problem. In fact doing so is a convenient method to avoid solving the problem. "It someone's or something else's fault so there is nothing I can do about it."

When something goes wrong for me, the first person/thing I blame is me. Then I go to work trying to make sure I am doing everything I can to correct the issue. If that fails, then I will start looking to point a finger. But honestly? Pretty much all of my issues have turned out to be self inflicted one way or another. You would be amazed how many times I have said WHAT WERE YOU THINKING!!!!!

[Rcnewcomb]

I checked the Onsrud chip load data for precision board (similar to duna). For a 1/2" two flute spiral O (52-704) they are running at 15K RPM and 300 IPM (5 IPS).

If you are running a regular two flute bit instead of an O flute then the suggested settings would be 18K RPM and 220 IPM (3.67 IPS).

Are those in the range of what you are running?

[Blackhawk]

Randall - Thank you for the links for HDU chip loads. I was running a standard 1/2" endmill at 2.2 IPS and 19,000 rpm. My chip load was .003, so a little on the lighter side based on the Onsrud charts. I have a PC router and older PRT alpha, so I tend to shade to the lighter side. Next time, I could at least bump that up to .004 or .005 and see if that helps. Neither the router or Shopbot was struggling at .003

Chemstock - I cut two similar signs. The first one actually cut with less tear out. On that one, I was using a flat bottom cutting endmill. It looked a little dull when I finished, so on this 2nd sign, I put in a much sharper standard plunge endmill. The plunge end vs flat bottom end could have been a factor.

[Rcnewcomb]

I have a PC router and older PRT alpha

My first machine was a PRT Alpha with a Porter Cable. You should be able to run faster feed rates if the router is set to higher RPM -- 20lb Duna should cut pretty easily. You will be able to hear if the router is struggling.

If you are going to cut a lot of this material then it may be worth investing in a spiral O flute bit. The larger gullet of the O flute helps with the material removal rate.

And the plunge vs. FEM would certainly explain the bottom finish issue.

[Blackhawk]

I think that I found the main culprit to my tear out problem. Chemstock got me thinking about my tools being sharp. I checked the 1/2" plunge endmill that I used on the 2nd sign and it had one corner chipped off. It was missing about a .010-.015" piece. I checked it before I used it and it was OK, but it must have chipped early on. That definitely explains a lot of the tear out and some steps that I had.

I did cut the first one with a different bit (1/2" FEM). I still had tear out, but only half as bad. That cutter was was not new and by the end of that sign it was not awful, but at the end of life. So, again dullness hurt me most likely.

I did play around tonight with stepover settings with the toolpath preview. Nothing that I tried really helped reduce the number of slivers and Z moves in the toolpath. The only big difference was changing to a raster pattern. That would have added an hour to the run time, but probably would have been worth it in hindsight.