Messy 'stepped' V-groove cut problem

[chubb]

Hi all,

I'm having an issue with a deep 90Deg V-groove cut I'm doing, and was hoping to get some opinions and guidance

It seems to be sort of 'stepping' inwards with each pass by about 1mm and creating a horrible stepped look to the cut rather than a smooth side. I've spent the whole day trying to figure it out (its 7:45pm where I am now) and just had to abandon doing any further cutting till I could figure it out.

I'm using the V-groove tool/wizard in Vcarve and have gotten fantastic results in the past but I don't even know where to begin with this problem.

Some Info.:

8 month old shopbot (PRSAlphe 120-60)
Spindle
Latest control and firmware installed.

Cutting Info.:
Cutter Bit - 90deg V-groove 1.25"D (Amana 45751)
Pass Depth - 0.25"
Final Pass Stepover - 0.75"
Clearance Pass Stepover - 1"


Attached are some photos showing the cut and the 'steps'.

Does anyone have an idea why this would happen or how to fix it? it's frustrated me to bits trying to fix it.

Thanks so much in advance for any help or ideas on how to solve, it's greatly appreciated.

thanks,

Mark

[Burkhardt]

I had a similar effect on a vcarve with a big 1.25" bit (not Amana but cheap ebay seller) lately. I suspected an incorrect bit angle, which should have been 60 degrees but took it to work and put on an optical camparator. The bit was exactly 60 degrees.

Turned out the bit had a bad grind on the side faces of the tip. pretty sharp and correct angle when looking onto the carbide blades but rather flat when looking along the blades, see below. That flat will dig an ugly groove. You can check if you have a similar situation.

https://lh6.googleusercontent.com/-R4d-2qSVt8w/UsYdBHcMesI/AAAAAAAAEeY/42UzN4ZuT3g/w570-h509-no/DSC02115.JPG

https://lh6.googleusercontent.com/-uzh6Hp4OSkw/UsYdCJ72BJI/AAAAAAAAEeg/T1Oui6FVFSY/w592-h518-no/DSC02116.JPG

[steve_g]

Mark…
As Gert has suggested, the most likely culprit is a bit that’s not the same as the one defined in your design software… another thing to consider is an out of plumb router but looking at your photos I don’t think that’s the issue.

Your final and clearance step-overs appear to be way out of range… Why would you have a step down of .25 and a step over of 1”?

SG

[chubb]

I had a similar effect on a vcarve with a big 1.25" bit (not Amana but cheap ebay seller) lately. I suspected an incorrect bit angle, which should have been 60 degrees but took it to work and put on an optical camparator. The bit was exactly 60 degrees.

Turned out the bit had a bad grind on the side faces of the tip. pretty sharp and correct angle when looking onto the carbide blades but rather flat when looking along the blades, see below. That flat will dig an ugly groove. You can check if you have a similar situation.





Wow. Spot on first time :eek:

Had a look at the bit and sure enough; looking at it with the cutters perpendicular to me it looks sharp as a pin. But looking along the cutters there was a pretty obvious flat tip about 1.5mm. Dunno how I didn't see it.

Not the quality I expected from Amana :mad:

Thanks for the response Burkhardt. You were absolutely right.

One more Q. Did you resolve the problem with a bit that was sharp from all facets?


Mark…
As Gert has suggested, the most likely culprit is a bit that’s not the same as the one defined in your design software… another thing to consider is an out of plumb router but looking at your photos I don’t think that’s the issue.

Your final and clearance step-overs appear to be way out of range… Why would you have a step down of .25 and a step over of 1”?

SG

Hi Steve,

Yeah, they are way out of range. I have set them to those values with careful consideration though :D and it's definitely not good practice.

When I have a mass of material to remove and a nice new sharp bit I usually would set the bit to a clearance stepover just less than the tool diameter. It clears out material faster. Because this work will be cut on both sides and cut through in certain places it also stops the program from trying to over flatten the bottom of the V cut with little time wasting steps when it will just be carved out when cutting the opposite side. Setting the Final pass stepover high also helps eliminate minor time wasting toolpaths without compromising on quality, and is set slightly above half of the tool diameter.

These little tweaks help turn an 8-hour job (in this case) into a 4.5-hour job.

I strictly only do this with sharp cutters.

I've attached a picture of a completed piece, although that ones about 4ft tall and the one I'm currently working on is 7ft. But they're exactly the same in design and layout.

regards,


Mark

[steve_g]

Nice work! Very similar to a lot of the accent wall hangings I do.

SG

[Burkhardt]

Not the quality I expected from Amana :mad:

Thanks for the response Burkhardt. You were absolutely right.

One more Q. Did you resolve the problem with a bit that was sharp from all facets?........

I suspect these bits are not really intended for CNC V-carving but maybe chamfering or making a single pass groove? In that case you would not notice the blunt tip.

For now I just used a 1/4" kyocera bit that is much sharper. I had hoped to save time with the bigger bit, going 1/2" deep in a singles pass. But, besides the cut quality, I can run higher feed rate with the small bit and the time difference is not that bad.

I may actually try a diamond hone to "fix" the big bit sometimes. Pretty useless as it is now.

[chubb]

Nice work! Very similar to a lot of the accent wall hangings I do.

SG

Thanks :)

Tha pain in designing and cutting such things seem worth it when a fellow shopper acknowledges your work :D




I suspect these bits are not really intended for CNC V-carving but maybe chamfering or making a single pass groove? In that case you would not notice the blunt tip.

For now I just used a 1/4" kyocera bit that is much sharper. I had hoped to save time with the bigger bit, going 1/2" deep in a singles pass. But, besides the cut quality, I can run higher feed rate with the small bit and the time difference is not that bad.

I may actually try a diamond hone to "fix" the big bit sometimes. Pretty useless as it is now.


You're probably right. I don't think they were meant for deep groove cuts. I was thinking about grinding them down as well but haven't quite figured out the geometry yet. It seems the cutting edges are slightly offset when looked from above which slightly complicates the grind.

Thanks for all your input Berkhardt. You've been a major help with figuring his out.

[joe]

Mark,

Your carved piece is excellent. Please tell us more about the design and how you'll be using this fine piece.

This may sound off course but I really like the effect your off-center bit produces. I may even have my bit grinder to the same to some of my V's. Or even better to buy some cheap HS bits and have a go at them on my grinder.

Thanks for posting. It's refreshing to see photo's of a problem posted. So often we are asked to solve a problems without them.

[tmerrill]

You can create the same effect without having a defective bit or regrinding one.

Calculate a vcarve or prism type toolpath using one v-bit angle but run the toolpath at your machine using a sharper angle v-bit. The pass depth set for the calculated toolpath will control the spacing of the resulting "steps".

In these quick examples the toolpaths were calculated using a 120 degree v-bit with pass depth set to 0.125" but run using a 90 degree v-bit.

I know this works with the Vectric software and would assume it would work with any software package that can calculate v-carve and prism type toolpaths.

Tim

[chubb]

Mark,

Your carved piece is excellent. Please tell us more about the design and how you'll be using this fine piece.

This may sound off course but I really like the effect your off-center bit produces. I may even have my bit grinder to the same to some of my V's. Or even better to buy some cheap HS bits and have a go at them on my grinder.

Thanks for posting. It's refreshing to see photo's of a problem posted. So often we are asked to solve a problems without them.

Thanks Joe,

The design for this piece was difficult. A lot of overlapping vectors and paths.

The client provided the MDF panels glued together and cut in a paisley shape (~30 pieces of varying sizes). Asked for a floral design with a simple border pattern.

Mapped all pieces using the probe tool.

Design was done in adobe illustrator, with consideration that it would all be carved using a v-groove cutter. Doing the design as a 3D object with one of the tapered ball nose bits to cut would have just taken waaaaaaaaayyyyyyyyy too long. V-Groove bit allows for mass removal quickly.

Designing it was the hardest part more than anything and getting the toolpaths right (V-Carve Pro doesn't like overlapping vectors and toolpaths). Also fixing it ina way that it could be flipped was also quite a task. Ended up using a form of registration marks.

This isn't the only work being done for the client. There were numerous border patterns of varying sizes and patterns and curves. I've added a photo of a small crown border that was particularly difficult coz it has a bow shape. The upper uncarved part is to be cut off with a band saw.

They're all for a traditional Indian wedding. Indian weddings are incredibly extravagant and immensely beautiful. The attention to detail and design is incredible. I never had any of my first design proposals approved, and not the second proposal, or third, got lucky on most with the fourth proposal :p

I would follow Tims technique with recreating the stepped effect. Much easier than the method I use. Will definately be using his method from now on :cool:

Thanks for the kind comments.

If you want to know any more you can let me know by PM or on the thread. I would post the .crv file so you could have a look at it and how it was done in VCarve Pro but its 24mb which is larger than the forum allows us to attach.