Pocket Tool Path problem in Vcarve Pro 9.518

[BWChester]

Hello Folks,

Haven't run the pocket tool path since prior to the 9.517 upgrade and the tool path ran good on this project. What is now happening when I compile the toolpath and run it on my CanCam D23Minitron, the 1/4 inch end mill does a complete first pass at the .125" depth then lifts the tool, goes back to the start point and puts a nice arch on the inside of the cut which is equal to the radius of my large clearance bit which is an Amana 1.5" diameter bit. It goes around and with the 1/4" bit and increases the radius of the inside of each corner to match the 1.5" diameter bit which is great but, after doing this on all passes to the final depth of 1", the tool lifts clear, moves back to initial start point and tries to hog out weird shaped corner at full 1" depth which causes the work piece to break free of the vacuum table.

I have run this project many times in the past and had no such problem. In previous versions prior to 9.517, the tool would make the initial cut then round the corners to the large area clearance tool and then continue to the programmed depth then retract to switch to the large area clearance tool. Why is it now trying to hog out this additional amount of material and why all at once?

Another interesting thing that is happening now with 9.518, the pocket tool path is leaving material behind. I am using a 90% step over on the large area clearance tool and it takes the full swath on the profile pass, then lifts, move to the center of the pocket, lower the head down to the desired cut depth then lifts again and goes to top of the pocket, does a jog to the upper left, back to center, jog to the upper right then back to center. From here it goes straight down to the bottom of the pocket does the angular jog to the bottom right, back up to center, then down to the bottom left then continues to the outside of the pocket, goes all the way around then lowers to the next depth and continues in this fashion.

I am using a raster at 90 degrees and a climb cut direction and profile pass is set to last. I must emphasize that the profile pass is set to last but it is doing the profile pass first. That in itself is not a real concern but would be nice to do it last as I want.

Sorry for the long winded explanation. What is going wrong? Could this be how Vcarve is calculating the tool path or is it how my machine is interpreting it? I am very confused.

[Adrian]

You really need to attach the file in question for issues like this otherwise it can be a bit of a guessing game.

[BWChester]

Hello Adrian,

Which file should I attach? I did attach the file showing the weird cut that is being added at the end of the 1/4" tool cut. Did you want the Toolpath file?

Thanks

Brian

[Adrian]

Hello Adrian,

Which file should I attach? I did attach the file showing the weird cut that is being added at the end of the 1/4" tool cut. Did you want the Toolpath file?

Thanks

Brian

The actual VCarve file itself. You attached a picture rather than a file to the previous post.

[BWChester]

Hi Adrian,

Sorry, but I can not provide the actual Vcarve pro file in a public forum as it is my customers proprietary design.

I could provide it privately with guarantees that it will not be saved or shared, however.

Brian

[TReischl]

What you could do is create something that also shows the issues you are having. Let's face it, pockets are not all that "proprietary".

In other words, draw a similar pocket, put it in a rectangle and away you go. That way you will get all sorts of help around here.

[BWChester]

What you could do is create something that also shows the issues you are having. Let's face it, pockets are not all that "proprietary".

In other words, draw a similar pocket, put it in a rectangle and away you go. That way you will get all sorts of help around here.

Hi again,

Never thought to create a new file. Been too frustrated trying to get this darned contract out and not thinking clearly.

Here is a sample file demonstrating most of what I mentioned above.

[TReischl]

Your stepovers are too large. Setting them to things like 95 and 98 percent is not a good idea and is not good machining practice. You are taking a huge stepover with a 1.5 bit but only cutting .0625 deep. You will be much better off stepping over a whole lot less, like 50% and taking a much deeper cut.

You may not like it, it may not be the way you think it should work, but stepovers that approach the diameter of the tool are a problem.

About the most I ever do is 75% when I am in a big honking hurry.

BTW, it was not "adding" any cuts at all, what it was doing is MISSING material.

[sharkcutup]

Make two Changes

1.) Change the toolpath order (Why are you changing the order after it is created? Just curious as to why you are changing it!)
2.) Change the stepover of the 1.5 dia bit to 50% to 75%

And I think this may solve your problem.

Sharkcutup

[Jan.vanderlinden]

Here's my take on the problem.
It is doing this because you are using a .25" cutter to get the desired radius in the corners and using an 1.5" clearance tool.
It is computing enough clearance for the larger radius of the clearance tool.
To prove this, I reduced the size of the clearance tool to .5' and the problem all but went away.
And yes, do your clearance cut first and reduce your stepover to 50% or less and your problem will go away.

Just my $.02

[TReischl]

Here's my take on the problem.
It is doing this because you are using a .25" cutter to get the desired radius in the corners and using an 1.5" clearance tool.
It is computing enough clearance for the larger radius of the clearance tool.
To prove this, I reduced the size of the clearance tool to .5' and the problem all but went away.
And yes, do your clearance cut first and reduce your stepover to 50% or less and your problem will go away.

Just my $.02

It is not caused by the relative sizes of the cutters. This is the geometry drawn to scale:

The issue is caused by the stepover being too large.

This is one of those cases where the intent produces unwanted results, like the .25 tool clearing out the corners when there is no need to do so. If'n I were doing it I would rough out the pocket with the large tool (I would NOT use a cutter that big, more like the .50 mentioned above) leaving about .015 material on the side walls and use a profile cut with ramping to finish the side walls. Might even leave .015 on the bottom if it is critical and then pocket with the .25 end mill at the end.

[BWChester]

Make two Changes

1.) Change the toolpath order (Why are you changing the order after it is created? Just curious as to why you are changing it!)
2.) Change the stepover of the 1.5 dia bit to 50% to 75%

And I think this may solve your problem.

Sharkcutup

Hello again,

I have been changing the tool path order to avoid too many tool changes. The job that this pocket belongs to has a total of 9 toolpaths and I try where ever possible to group my like tools together. For instance, I have to use a plunging round-over bit to smooth the top outside edge of the project, make two 1/8 inch screw mounting holes, then use the 1/4" bit to perform multiple operations as:
- create three pockets,
- Cut out the top of the piece (it's 1.5 inch thick)
Flip the piece over and while still having the 1/4" bit installed
- Cut the initial pocket outline,
- cut in two side channels
- cut out the bottom of the piece
Now I can change bits to the 1.5" clearance tool and finish the pocket .

Also, I have been using the tools available since the customer will not pay for new bits and provides only what he has. Excessively tight budgeting on a shoestring. Not a great situation but.....

So as some of you have mentioned, I have changed the stepover of the 1.5" and made it the only tool on the pocket tool path, introducing a new internal cut with the 1/4" bit. This seems to work in Vcarve Pro preview but can't test it yet as my controller chose this as a perfect time to pack it in. Hopefully I get the new controller working early in the week.

Thanks to all for your suggestions and tips. It is appreciated far more than I can put into words.

Brian

[sharkcutup]

Thank you kindly for the explanation! Makes sense!

It was just that I was wondering why you would change the toolpath order because of it being designed to work the other way -- Clear cut the pocket then clean up the edge.

Thanks again for taking the time to explain your process and why the toolpath order change!

Sorry to hear about your controller

Sharkcutup

[Jan.vanderlinden]

While I understand your explanation and drawing, why is it that when I reduced the clearance cutter size the problem went away?

[TReischl]

While I understand your explanation and drawing, why is it that when I reduced the clearance cutter size the problem went away?

For the same reason the problem goes away when the stepover is reduced.

The reason I wrote that it is caused by the large stepover is that will almost always cause the error no matter what the size of the tool. I can easily produce the error with a .5 diameter end mill, just give it a 98% stepover and try a few different sized pockets. This is not the case when the stepover is set to lower values. So, it is not the tool diameter.