Flatbed cutting latex ink and PVC, weird edges?

[MGB_LE]

We just installed an HP R1000 latex printer to supplement our HP Latex 570. We were doing some prints on 1/8" and 1/4" Sintra, aka expanded PVC. Our Colex flatbbed cutter cnc, yielded some not so clean edges. We had to go back and peel away the wavt, stretched edges of the print, or use a razor blade to clean up the edges. We tried clockwise and counter-clockwise routing. Both methods exhibited the problem to varying degrees, so we went with the least problematic direction.

How can we get better results with less "cleanup" or manual intervention needed? The router bit was

new.

Below is the router bit info:

T00502 Upcut Router Bit​

Bit Type	Upcut, 1 Flute
Cut Diameter	6mm/ 0.236″ -approx 1/4″
Cut Length	12mm/ 0.472″ -approx 7/16″
Shank Diameter	6mm
Recommended Use	Soft & Hard Plastic, Acrylic, Di-Bond, Wood​

 

[WYLDGFI]

We use a 500 bit on our gator foam I believe. Just looked in our kit....502 isn't in there for us.

 

[Raum Divarco]

Materials all come down to a variety of factors.
Some sheeted materials like this will lift away from the bit as it is cutting.
This means the top layer will be rubbing against the shank more than being pulled in to me mulched away in the cutting process.

you have 4 options that are typical for any application
- cut from the back on one sided prints and add to the cycle time
- use a down bit to avoid these problems all together at the cost of a slightly less clean edge.
- chase the top edge of the dieline with a knife tool prior to router cutting so that the fault line you create will always be clean
- knife cut the 3mm pvc pieces whenever you can from the front or back. double sided blade is plenty durable.

 

[letterworks]

Some PVC is just like that, I have certainly seen that edge before but not often. I think it's a manufacturing error in how the skin is formed.

But, in general a downcut bit or a knife cut first, as recommended above, should work, upcut bit for the bottom edge ideally.

Sandpaper block might take off the crap better than trying to cut it too.

 

[jimmmi]

This looks like burned from high rpm. How many rpm you use? By the way, use a two flute straight cut and always have clean edges

 

[MGB_LE]

This looks like burned from high rpm. How many rpm you use? By the way, use a two flute straight cut and always have clean edges

We were running at 24,000 rpm.

 

[Josh Martinez]

What is the max RPM of your spindle? We have customers using the XR2062M-CBmm This is a 6mm tool with a 25mm cut length. This tool has 3 flutes low helix which will help with top cut quality. The customers run tool 24,000-36,000 RPM at 200 to 300 IPM. Hope this helps. https://www.xedgetools.com/product/xr2062m-cb-6mm/

Josh

 

[letterworks]

I continue to think this is just a problem of crap sheet (maybe due to PVC supply issues), not a cutting issue per se.

Grab a scrap of old pvc and cut that and see?

 

[jimmmi]

We were running at 24,000 rpm.

24000 rpm is way too much. I cut pvc with 12000-14000. Its like you have too many rpm and slow feed rate. Try to find the correct feed rate with lower rpm.

 

[MGB_LE]

What is the max RPM of your spindle? We have customers using the XR2062M-CBmm This is a 6mm tool with a 25mm cut length. This tool has 3 flutes low helix which will help with top cut quality. The customers run tool 24,000-36,000 RPM at 200 to 300 IPM. Hope this helps. https://www.xedgetools.com/product/xr2062m-cb-6mm/

Josh

I’m not sure the maximum spindle speed, but it may be 24000rpm on our Colex Sharpcut.

 

[ThuddNugget]

Stupid question: Have you tried reversing the milling orientation?

 

[MGB_LE]

Stupid question: Have you tried reversing the milling orientation?

I'm not certain if my operator tried reversing orientation. I have a leftover printed piece from the job that is waiting for experimentation. Funny thing though: he's just one guy and actual jobs leave little time to just try stuff.

 

[MGB_LE]

Stupid question: Have you tried reversing the milling orientation?

The only stupid question is the one we didn't ask! Questions are awesome.

 

[kerwinchua]

We just installed an HP R1000 latex printer to supplement our HP Latex 570. We were doing some prints on 1/8" and 1/4" Sintra, aka expanded PVC. Our Colex flatbbed cutter cnc, yielded some not so clean edges. We had to go back and peel away the wavt, stretched edges of the print, or use a razor blade to clean up the edges. We tried clockwise and counter-clockwise routing. Both methods exhibited the problem to varying degrees, so we went with the least problematic direction.

How can we get better results with less "cleanup" or manual intervention needed? The router bit was View attachment 155743 View attachment 155744 View attachment 155746 View attachment 155748 View attachment 155749 new.

Below is the router bit info:

T00502 Upcut Router Bit​

Bit Type	Upcut, 1 Flute
Cut Diameter	6mm/ 0.236″ -approx 1/4″
Cut Length	12mm/ 0.472″ -approx 7/16″
Shank Diameter	6mm
Recommended Use	Soft & Hard Plastic, Acrylic, Di-Bond, Wood​

Try putting two layers of pre-mask or transfer tape on the face (I believe you cut these with image side down) then using a caliper measure the thickness with the pre-mask on. Say for example if it reads .45” tell your machine to cut .44” only. This will clean your edge all the way and leaving the fuzz on the pre-mask which you will remove anyway

Let me know if this works

 

[Spen101]

The only stupid question is the one we didn't ask! Questions are awesome.

I don't believe this was asked yet, do you know how many passes were used to cut through the piece?

I'm fairly new to this stuff, our shop acquired a Sharpcut a few months ago. But I usually do 3 passes at around 300ipm for 1" PVC board. It may put stress on the softer core if the feedrate is too slow, but I find I this gives me the smoothest results on all edges (particularly when vinyl/premask is on the face, facing down).

I'm not sure if you know much about the operation of the software, but setting the height of your last pass in the "Depth Final Pass" section will allow you to use that final layer to be used with the Cleaning Path option (near the bottom of the tool parameters, disabled by default), I have my settings at 10-15%. Sometimes the cleaning layer option really helps (especially for acrylics).

I would always account for an area of space on your workpiece specifically for running a test cut, to allow for a few different parameter tweaks. Especially important for new material configurations, as it saves a lot more time than it does to clean up choppy work.

Also make sure your bits are perfectly clean before starting, and I like to add a bit of lubricant (which is usually used for the colex itself) to the bit.

Almost any time vinyl is involved with the router module, it tends to cling to the bits and may start compromising cut quality partway through.

It is a good machine, but having a clean carpet is imperative to getting your tool measurements right the first time.

Happy Halloween

 

[MGB_LE]

I don't believe this was asked yet, do you know how many passes were used to cut through the piece?

I'm fairly new to this stuff, our shop acquired a Sharpcut a few months ago. But I usually do 3 passes at around 300ipm for 1" PVC board. It may put stress on the softer core if the feedrate is too slow, but I find I this gives me the smoothest results on all edges (particularly when vinyl/premask is on the face, facing down).

I'm not sure if you know much about the operation of the software, but setting the height of your last pass in the "Depth Final Pass" section will allow you to use that final layer to be used with the Cleaning Path option (near the bottom of the tool parameters, disabled by default), I have my settings at 10-15%. Sometimes the cleaning layer option really helps (especially for acrylics).

I would always account for an area of space on your workpiece specifically for running a test cut, to allow for a few different parameter tweaks. Especially important for new material configurations, as it saves a lot more time than it does to clean up choppy work.

Also make sure your bits are perfectly clean before starting, and I like to add a bit of lubricant (which is usually used for the colex itself) to the bit.

Almost any time vinyl is involved with the router module, it tends to cling to the bits and may start compromising cut quality partway through.

It is a good machine, but having a clean carpet is imperative to getting your tool measurements right the first time.

Happy Halloween

Sorry that I'm just seeing this post. We usually cut print side up. This material was 6mm thick, so one pass. Curious about what type of lubricant you use on the bit. I'd say our bits are clean when swapped in. I need to experiment with using a knife first to score the latex ink, followed up by routing.

 

[balstestrat]

Sorry that I'm just seeing this post. We usually cut print side up. This material was 6mm thick, so one pass. Curious about what type of lubricant you use on the bit. I'd say our bits are clean when swapped in. I need to experiment with using a knife first to score the latex ink, followed up by routing.

You don't need to score the ink... It's the top layer of the material you are scoring if anything.
I mean you can cut that same stuff without ink and it should behave exactly the same. The ink shouldn't make any difference being on the top.

 

[Spen101]

Sorry that I'm just seeing this post. We usually cut print side up. This material was 6mm thick, so one pass. Curious about what type of lubricant you use on the bit. I'd say our bits are clean when swapped in. I need to experiment with using a knife first to score the latex ink, followed up by routing.

No worries! Since it is an upcut bit, what you might be seeing is the vinyl being pulled up and away from the material. I highly recommend that, if you must cut the the graphics facing up, to use premask tape on top. If you are cutting this way then you would definitely not want to do multiple passes.

We have had the best results running everything premask + vinyl side down. The upcut nature of the bit will actually influence the vinyl to stay neatly along the material. To ensure this works best, I usually run two passes. One to cut through most of the material, leaving around 0.02" - 0.03" for the last pass; that way, there is the least amount of drag possible for the cut which includes the vinyl face.

I highly recommend just running a test to see if this works with that orientation. I also suspect your feed rate is too slow, based on the amount of fraying/feathering along the middle core part of the material, visible in your images. One pass at too slow of a feedrate could be creating a buildup of melted PVC, adding another factor for rough edges and drag against the vinyl. I suggest at least 300 ipm (ours is set to 350 ipm) in two passes if you're going to run it at 24000rpm.

 

[johnnysigns]

We usually mount polyester vinyl like that with some heat assist and fairly slow on PVC which can be pretty low surface energy depending on the brand. Have you tried a downcut bit?

 

[rx7boy]

we also just received our new R1000 and I just cut some 3mm and 6mm palight pvc. And did a quick test and had the same as you but then realized the bit was old. Switched to a new bit and it cut super clean, no finishing afterwards whatsoever.