Looking for advice with this file in Estlcam

I was showing my friend some of the pieced I’ve cut and he asked if I could cut him a sign for the horse carriages he sells. It’s a pretty straightforward design so I told him I’d work on it. I’m still pretty new at all this so I’m looking for help.

[attachment file=35536]

I’ve figured out one way to carve the letters with a V bit and carve the curve with a 1/8 and 1/4 flat end mill then cut the whole piece out, but I was hoping someone could help me with a different way. I think I’d like to carve down the background so the letters, the curve and the small strip around are all uncut, and everything around is cut into the piece. I thought this would be pretty straightforward where I could create holes and parts then surround everything and make an island. I think that would work, but to do that and get the detail I need I think I’d need the 1/8" bit. I can only go max 24" square right now. Besides taking forever, I don’t currently have great 1/8 bits and they tend to break so I don’t know that it’s even possible.

Then I thought that I could use my 1/4" mill to bulk cut the big open areas and then fill in with the 1/8 mill around the letters. It’s getting a bit too complicated for my novice skills. Am I on the right track or is there a better/easier/more efficient way? Is there a different bit that I’d need to do it a better way? Would I get a good finish using a (quality) 1/8" bit?

[attachment file=35537]

The screenshot shows me in the middle of the process of cutting up the large areas for my 1/4 mill. I can’t seem to get the island function to disregard all the areas that I’ve already milled with the 1/4" mill. This results in a 5:30 cut time, most of which would be the 1/8" mill running in air. I suppose I might be able to modify the G-Code to eliminate some of this, but I thought I’d check here for better advice.

Thanks in advance for your help!

Have you seen this carve video:

It looks like you can pocket with the 1/4" and then carve with the v bit, to a set width. Maybe?

I believe Jeffeb3 is correct, set a “maximum carve” value on the carve. This should force the vbit to stick to the edges. Then pocket with the flat bit.
Post a pic of your result!

Thanks. I had seen that video but since I didn’t need it when I watched it the info didn’t stick.

I didn’t have much luck with the carve/pocket but I’m still going to try things in the program before cutting.

[attachment file=35606]

Right now I’ve cut out large areas with 1/4" bit for pocketing and the 1/8" bit will do areas in the letters.

I’m pausing on this until I can get a 1/8" bit I can trust. The current ones I bought are very brittle and I don’t trust them. I also need to work on my tool changes. If it isn’t exact the cuts won’t be at the same level.

Maybe in the mean time get some dense foam insulation and do some test carves to get it dialed in before you waste and wood and break bits. Can’t wait to see how this turns out.

So I finally feel your pain. But there is an easy solution. I upgraded to estlcam 10.039 and there is an option on carves to choose a pocket tool. So you can choose your 1/4 or 1/8" bit and let it figure the rest out. It seems like to do that, I had to put in a 100mm or something else huge into the max carve width box.


use the “Carve pocketing tool” option:

[attachment file=37025]

Best workflow:
[li]Select the Carving tool[/li]
[li]Create all Carves[/li]
[li]Select all (Ctrl + A)[/li]
[li]Set an appropriate depth limit[/li]
[li]And finally select the flat bottomed carve pocketing tool[/li]




Thanks. I had updated once I figured the carve pocketing feature, but I forgot to come back to this thread. I’m now using a 1/4 V bit for the carves and 1/4 mill for the pocketing. They’re all outside carves. I’m going to try cutting it this weekend.

The piece I was missing up to now was selecting them together. I didn’t realize that this groups them and reduces the number of tool changes.

The only issue I had is with the carves on the small letters of “Carriages”. You can see for some reason it was cutting the tops of the Rs and Is. I was able to get around this by manually tracing the carves around the letters. The key was not to start the carve trace in a corner, but along a flat edge of the letter.

[attachment file=37035]

1 Like

Sry, double post.

I can’t wait to see this carved. Good luck!

Thanks, Christian.

[attachment file=37101]

It worked pretty well for me. The tip of the bit broke off pretty quickly, and then broke a few more times, but other than that, it was smooth sailing, and this Beer Bear carving was about 10 mintes. It’s 5x4in.

I was playing around yesterday with a previous version that didn’t have that, and it was quite difficult to get the same effect, and it ended up doing a lot more carving than it should have. This is a great feature.

I posted early (and even got a reply!) but it’s disappeared. Here’s the finished sign. It’s the one on the bottom. I’m still looking for ways to clean it up. It looks good from 3 feet away but if you get closer it’s a bit messy. Changing between the 1/4 flat and 1/4 v-bit is creating some mis-alignment.

[attachment file=37520]

I’m still having problems with tool changes. I posted in another thread about that. (Hopefully it didn’t disappear.)

Just curious but did you run the pockets first or the v-bit? If you ran the pockets first you might try the v-bit and then the pockets. Might ensure your letters are correct and then you can clean up anything missed in the pockets. Also for small areas you might consider a 3rd tool and clean up with an 1/8" flat in the small areas. And also on the vbit pass are you doing a rough cut and then a finish pass? Might help with the clean up a bit. And then you might set the pocket with the flat mill slightly deeper than the vbit and that might help with some of the ghosting as long as the flat endmill can get into the corners. Which might be a reason to do both 1/4" and 1/8c flats for the pockets to clean it all up. Just throwing ideas out there. I will be doing this same learning curve once I get mine running in a few weeks.

Right now it’s doing a carve withe 1/4" as the pocketing tool. First, it does the 1/4" then it does the V-bit. I don’t think there’s a way to do that the other way around using the carve. The carve tool won’t allow me to setup a finishing tool, so I guess that’s not available. I haven’t used the finishing option on a project yet.

I’m going to change my tool change procedure and I’m hoping that will help with the cleanup.

When you select a “carve pocketing tool” and have to switch from a vbit to an endmill, how does the software allow you to change the bit? does it go back to origin and just stay or…


There’s a couple of ways of doing this. This is how I do it:

I put the gcode for the two bits in two separate files. I manually set my ‘0,0,0’ point on the machine. then I use two clamps on the X and Y gantry to create temporary end stops. I run the first gcode file. Turn everything off. switch bits, pull the z axis back to where it’s touching the two clamps, and then turn everything on and run the second gcode file. I find the hardest part doing it this way is getting the Z height back to an identical 0 starting point, but it’s usually close enough.

I know this is an old thread but trying to understand this. How do you put the gcode into separate files?

I use F360.

I post process each toolpath separately. I rename the file before saving.

When I used ESTLCam, I would save the ESTLCam file separately for each tool. Then when I ran the post processor in ESTLCam, it would only process the one file.