I have the X-Carve 1000mm with the 300w spindle and the end mill starter set. I have yet to complete a good carving job because I am a total NEWBIE to this. I bought V Carve Pro with my X-Carve and the settings are overwhelming to say the least. I have gone through lots of wood in the garage trying to carve something nice and I can see where it would be easy to get discouraged and lose interest in this whole new concept.Easel is easy to use but matching up the bits to the job is information overload to a point. UGS has already busted my Z axis micro switch because I forgot to change from IN and MM when homing.
Everyone on this Forum is knowledgeable and very helpful, so I was wondering if the veteran CNC folks could take the time to post a successful carving project with the bits they use the type of wood the spindle and the feeds and speed and depth of cut they use to complete the job even if it is just a letter on a piece of scrap wood, just something us new folks could try to copy and get the feel for this whole new adventure without getting discouraged to the point of giving up.
Any help and sharing of information for us new folks would greatly be appreciated
Vcarve is an excellent piece of software. I suggest you be sure you have the clipart downloaded and then pick one of the 3D examples and carve it to see what can be done.
I started a new project, set my material to 5 inch high by 5 inch wide and .5 inch high. Then when to the clipart/animals folder and copied the eagle to the workspace. (be sure the X/Y zero is set to bottom left corner, for some reason it defaulted to middle)
Then move to the toolpath menu (on right side). Select the eagle model and then click the rouging pass tool. I used a quarter inch endmill for the roughing with 20 inch/min feed and DOC set to .07 (I am getting a lot of chatter if I make a deeper cut each pass with the quarter inch tool). the default setting are fine. Calculate the rough toolpath, then click the finishing tool. I selected a one eighth roundnose bit for the detail pass with 30 inch/min feed and a DOC of .06. Again the defaults are fine, so calculate the detail toolpath.
Save each toolpath (changing the extension to .NC). and run the rough and detail files from UGS
Be sure you have a good zero position you can find again in case you move the spindle during the tool change.
I used a piece of cherry and here is what it looked like after staining
I probably should have used a .0625 roundnose bit for the detail pass to make the cleanup easier, but overall I was happy with the project and Vcarve.
Allen, now that’s what I’m talking about. Great info and something to look forward to carving. I did load the clipart when installing V-carve. I need to do some BIT research and invest in a better variety so I can do these things. Question: I downloaded the V-carve post processor files for the Xcarve and send them to UGS. Is that Ok or should I change that to something with NC extension? And when you have a tool change does the carve job just stop to switch the bit and then you have to hit a restart button or something?
Thanks again for the info it’s just what I was looking for. I plan on keeping a notepad handy and keeping notes when I get something to work like your above carve.
The X-carve post processors (inch and mm) work great. i always use the inch version. The only reason I change the extension is so that UGS will see the file when I click the open and browse in UGS.
[Note: I create the toolpath on my desktop computer that is running V-Carve. I have V-Carve set to save the toolpath files to my dropbox account, then when I am in the shop I can have my CNC laptop use UGS to open the files directly from dropbox, I was having to physically copy the files to a thumb drive and transfer them that way but using Dropbox is so much better.}
The gcode created from V-Carve will return the spindle to the X/Y zero with the Z at about 2 inches above the work when the rough job is completed. Then I just power off the spindle (leaving the motor power on) and change the bit (trying not to move the spindle X/Y). Then I lower the new bit to just touching the work surface, load the next gode file, zero all three coords and send the gcode.
I recommend that you get a roughing bit and detail bit with the same shank size so you do not need to change the collet with each bit. (my quarter inch bit has a quarter inch shank, and the 1/8 inch detail is a 1/8 inch shank so the bit change requires a collet change)
I also recommend you get a 90 degree Vbit and a 60 degree Vbit if you do not already have them. V-Carve does an excellent job of lettering with those bits.
Nice eagle! When carving a 3d path the BIGGEST ball nose that is capable of cutting the design the better for clean-up because it creates a smaller scallop. Here is a great article about adjusting step-over and choosing the appropriate sized cutter: http://www.cnccookbook.com/CCCNCMillFeedsSpeedsStepover.htm
I just cut a bass with a 1/4" ball nose and it came out better than my eagle head done with a 1/8"… that is until my system crashed thanks to a power surge.
Thanks for the tip, I expected exactly the opposite to be true. But now that I think about it, I can see how a larger tool would reduce the tool marks.
Any advice on how to orient the grain when doing a 3D cut like this, I am sure it must make a difference but I do not have enough experience to know how to figure it out.
Nope. Still experimenting. I had the grain follow the side of the bass and it was SO cool… until it crashed. There is no real way to finish it now. I do like the contour toolpath better than the raster for organic shapes. If was cutting something very geometrical like nested rounded over squares, I would probably go raster.
I went to a furniture store the other day and they had carved fish on the wall for $50. They looked like they were painted by a child. Now I am obsessed with carving fish.
Good stuff guys, can you throw in some links for the bits you are using? Another information overload subject there.
Here is a link to the 1/4" ball nose I use. I don’t know where I got my 1/8" - probably from precisebits.com.
I have been purchasing my bits from China on Ebay. Most ball nose and fish tail bits are less than $10 including shipping.
So far I have been very pleased with the quality of the bits, the shipping takes about 2-3 weeks so that is a downside, but the price is the selling point for me.
Thanks for all the good info guys. I never thought there would be so much to carving a piece of wood with one of these machines. I’m still trying to compile information and put a bit shopping list together and trying to get something going.
Please keep it coming.
I have attached a basic Feed and Speed calculator I found (Excel format). It allows you to enter your feed rate (celll D4) and it will calculate the RPM required to produce various chip loads.
The spreadsheet also shows the recommended chip size for various materials with 4 different size bit diameters.
I added a column to show the Dewalt Speed setting necessary to achieve the desired RPM. If the required RPM exceeds the 27,000 RPM limit of the 611 it will display “To Fast”. If the required RPM is below the minimum speed of 16,200 it will display “To Slow”. Otherwise it will display the speed setting between 1 and 6 (i.e. 2.5 is halfway between 2 and 3)
The first thing I noticed is that if these calculations are correct, I have been running my RPM’s way to high.
For example if cutting hardwood with a .125 inch bit the recommended chip size is between .003 and .005
To achieve that chip size with a two flute cutter moving at 100 inches per minute the RPM should be 16,667 or a setting of about 1.5 on the Dewalt 611.
For MDF with a Feedrate of 125 inches per minute and a .125 cutter the Dewalt should be set at 1
Please let me know if anyone finds an error with the calculations, they look pretty straight forward but wow these numbers are very different from what I have been using.
CNC Speed Calculator.xlsx (14.0 KB)
Thanks for posting this. I feel like I’m still guessing a lot with feeds and speeds. Hopefully this helps. I may be doing some carving later. I will use the chart and see what kind of results I get.
@Allen Massey - above where you say, change the bit and try not to move the router… Mine is set to lock the motors when it is stopped… It would be very difficult for me to move the router during bit changes. The setting in grbl is $1=255
Thanks Erik, Mine locks also, but when applying torque with a wrench to loosen the collet it is easy to overcome the holding power of the motors if I am not careful.
Cutting some pine this morning with a 4 flute 1/4" endmill, I slowed the Dewalt down to about 2.5 and it is cutting much better, I am running at 70 IPM and I am getting nice clean cuts. Thanks Allen.
Do you have the nema 17 motors or the 23s? With the 23s locked I am in no danger of moving it while I am changing bits. It is solid.
I am still using the nema 17’s. It may be time to upgrade.
I’ve noticed it is always time to upgrade something
Wow, that speeds calc is great but I’m a bit scared to try 300inch/min for hardwood with a 1/4" cutter! That sounds super fast - I wouldn’t think the motors or belts could cope with that? I’ve been using 40inch/min and the router set on 5 so far, so I should probably push that up a bit.
I agree that 300ipm is to fast. So what I try to do is use a smaller bit or if possible a bit with 1 or 2 flutes.
But yes, I was running my 611 way to fast for the feedrates, Lowering the speed helps a lot. I have also been increasing my feedrates to between 90 and 120 ipm (up to 140 on soft woods and MDF)
I was very surprised by the number the calculations were providing but they seem correct, The only “non calculated” number is the chip load and those seem very consistent with the values most bit manufacturers recommend.
I would like to find a source of chip load values for 1/16 and 1/32 bits but so far I have not seen any published numbers for bits that small.