You have two issues the first is the plastic. Do you know what type of plastic? The general rule of thumb for plastic is to go faster to make chips rather than strings or melting. How is it being secured to the MDF as lifting of the plastic could make the other issues worse. I’ve been very happy with painters tape and CA for thin sheets. The second issue is limiting the depth of cut on a V-carve tool path. The tool is probably not allowed to go deep enough to have to top edges show the proper geometry. With the need for limited depth of cut Advanced V-carve is the way to go as it will create extra tool paths to get the proper shape regardless of the depth restriction.
I know its Rowmark engraving plastic and I’m using Rowmark Fat-Mat engraving table hold down mat. Which does work well in holding the plastic down.
For the End Mill I have done different speeds and different feeds but there is still a very high chance there is either plastic build up or it just breaks. We have a pack of .6 mm end mill bits because they break so often. Which is why I am trying to just use the V carve we have. The plastic is only 0.06 inches deep.
I assumed the program would be able to adjust for the geometry of the bit when I put in the depth. 
I did try the Advanced V carve but without using the End mill bit. It left an outline and does not carve out the whole letter. (shown in the example picture)
This might be limiting depth in simple vcarve. A simple vcarve goes down center of letters until the vee bit touches both sides of the line. Switch to advanced vcarve to limit depth. Advanced vcarve goes around outside of letters instead of down center.
When a simple vcarve use bottom of material when possible. However on thin material you can cut through so use advanced vcarve to limit depth of cut.
The “bones” effect is classic to limiting depth of simple vcarve. The bit cannot touch both sides of line with depth limited.
How does that compare to the 3D preview in Carbide Create?
Looks as if you’re overcutting some corners, and not clearing others — debris on the tool?
Hi, So I have this happen to me when I use the vcarve option and I’m doing thicker lettering (so the carving has to go over one side of the letter and then other side. One thing that resolved this was to use the advanced vcarve option in CC. One other thing that could help is the depth of cut. Try making the depth of cut more shallow.
When I make the cut shallower on advanced Vcarve, it just gives me an outline. (the ASC one)
You can see on the top N that it didn’t quite get all of the inside, which is why I went deeper.
Did you use a pocket bit for the first step on the advanced vcarve?
From left to right, all on the same size rectangle:
- A VCarve to full depth
- A VCarve with limited depth
- Advanced VCarve, no clearing bit
- Advanced VCarve with clearing bit
Setting a depth for a VCarve sounds like a thing you might want to do, but the reality is that the result is never what you want. The right way to limit the depth of a VCarve is to use a V bit with a larger angle.
For the lettering you need to do, does if have to be this font? The best way to create very shallow letters is either Advanced VCarve with a very small clearing bit, OR use a font that allows you to just use an endmill for the whole thing.
For example, the oddly named “ZnikoSLSVGinOT-8” font is font that is EXTREMELY skinny, so you can carve using an endmill using a No-offset Contour:
In CC, using 1" tall letters and a 1mm endmill, it would look like:
In this picture, the bone is about 1" across the middle section, letters carved using a 1mm endmill:
Unfortunately it does have to be this font. That is what the customer wanted.
I can do the lettering with a just small end mill.
Top one is cut with the endmill. (not send-able because it had a noticeable scratch) Bottom one was cut at a too fast feed speed causing it to chip.
.5" Arial Lettering
I was just trying to avoid using an endmill because at the size I need, the endmill either gets covered in plastic or breaks. Its only a .6 mm bit. I’ve broken so many trying to get the settings right where it doesn’t break or have plastic build up. Slower/Faster Feeds, Slower/Faster Speeds, setting the depth as shallow as possible. I don’t really want to have to baby-sit this machine while it cuts for hours. (neither does my boss)
I was hoping I could just use a V carve but it seems like that it not going to be a solution.
Have you tried REST machining? (available in Carbide Create Pro)
I am not sure what that is. We only have Carbide Create V6, we do not have the pro.
vcarving “small” details in plastics often turns out to be a pain in the neck. That because most of the cutting work is done by the tip of the Vbit, and at the tip itself the cutting edge has a speed of ~zero, so it’s not really cutting, still it’s moving so it’s not unusual to end up with small chunks of melted plastic at the bottom of the V grooves, which then have to be manually cleaned up (not fun/efficient)
If you had good success with 0.6mm square endmills, I would advise to go down that avenue again and “just” fix the breaking/melting issue. Are you using a single flute endmills? They are just superior to anything else when it comes to cutting plastics (simple reason: one flute = much more space for chips to evacuate = much less likely to clog the flute/recut chips and get melted plastic), and once you dial in the feeds and speeds and depth per pass, you can run them for hours with no breakage in sight
Check out this example 1/32" single flute from Amana
Using good dust collection or an air blast (even better) goes a long way to avoid chip recutting/melting too.
And plunge FAST. If you see strings of plastics wrapping around your endmill, it’s not unlikely that you are plunging slow, which leads to partial melting during the short time of the plunge.
With good feeds and speeds, you should get lots ot teeny tiny plastic flakes, and no strings/melted plastic
The one I was using has 2 or 3 flutes.
We do have some O flute that work great but none that small. That small O flute would work perfectly. I didn’t know they did make them that small.
I did add a dust collector, which helped a lot keeping the bit from getting hot. I did try to suggest getting an Air blast. I think that would most likely be the best solution (along with the tiny o flute). Would you have any recommendations for air blasts? I think at one point they bought one for CNC but I know it’s supposed to be used with oil and not air. I could not rig it up with the air hose.
I’m not plunging very far into the plastic, only .006" majority of the time since I only need to take the top layer off. Though I will try changing the plunge rate.
We had a long thread about this:
Most people seem to use the Amazon variety of air blast, which works fine but requires a good air compressor. I was quickly annoyed by the sound they make (even the quiet ones), so in the end I went for using an airbrush compressor (Amazon again) and it has been working great for me. All details in the thread.
To the OP, see the last 2 images here… You are getting the 3rd one in and I believe you want the 4th one in, see Mhotchin’s note about that and you may be good to go? Also the stuff Julien said 
You could speed things up a lot using the Pocket / Contour trick. You can pocket with a larger bit, then run a contour using a smaller bit to get the details.
In general, if the smaller bit is at least 1/2 the size of the larger bit, then the result is the same as if you had pocketed the entire region with the smaller bit.
Since the bit you are using is 0.6mm, you could instead pocket using a bit up to 1.2mm, then just do an Inside Contour using the 0.6mm bit.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.