Cutting too deep!

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro

Cutting too deep!

Postby Yabba » Thu Mar 28, 2019 7:39 pm

Hello everyone. I can't seem to figure out what I'm doing wrong here... I am making trivets, and for some reason, the end mill to cut out the circles is cutting a good inch too deep. If anyone has a moment, please have a look at the file.

https://drive.google.com/file/d/15KSp-3 ... sp=sharing
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Rcnewcomb » Thu Mar 28, 2019 7:58 pm

The job was setup expecting you to Z-zero on the Top of the material. Did you set Z-zero on the spoilboard instead? That would cause the behavior you describe.
Zzero.JPG


Also, on both toolpaths you have checked "Project toolpath onto 3D model". Since you don't have a 3D model you should not check that.
Project3D.JPG
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3505
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Cutting too deep!

Postby Yabba » Thu Mar 28, 2019 8:12 pm

Thanks, I'll uncheck that selection. Yes, I do zero out on top of the material. Could there be anything else causing it? I do the vbit first, and it is fine. Once I change tools, everything goes nuts... it cuts a hole in the middle of the trivet, then goes to the outside to mill, but cuts way too deep. I would say close to an inch too deep.
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Leo » Thu Mar 28, 2019 8:28 pm

Did you reset the Z zero on the second tool?
Imagine the Possibilities of a Creative mind

www.leosworkshop.com
User avatar
Leo
Vectric Wizard
 
Posts: 2931
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: 1300 x 1300 x 254

Re: Cutting too deep!

Postby Yabba » Thu Mar 28, 2019 8:31 pm

Yes, I reset the Z on top of the material. I can't think of what I could possibly be doing to cause this... I've done similar cut outs that have worked fine, and can't see anything different in this one. I've tried this a couple of times now, even started the project from scratch... still doing the same thing on the cut out (2nd tool). If I had hair, I think it would be gone by now :cry:

I have to think that the issue has something to do with either the tool change or something silly I've done in the original setup with the toolpath or possibly even with my tool database?
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Rcnewcomb » Thu Mar 28, 2019 9:45 pm

I noticed the end mill is tool number 9. Is that a valid tool number for your setup? I've worked with other control systems where only certain tool numbers were valid.
Are there any special offsets stored for tool number 9? Does using a different tool number change the behavior?
Is it possible the tool is slipping in the collet? Have you tried a different end mill?

BTW, the stepover is set to 98% which will probably cause some problems with pocketing in the future. I'd recommend something closer to 40%-50%
Tool9.JPG
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3505
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Cutting too deep!

Postby Yabba » Thu Mar 28, 2019 10:01 pm

thank you, I'll change the step over. The reason I gave each of my tools a different number is that i had an issue once with a project where the software said the tool number was the same but the geometry was different... I had all my tools numbered as 1, so I changed them all to different numbers. Other than that, I don't know what the tool number actually signifies. All of my tools are from Amana, and I used the information they provided to set up each tool in the database. This is the second end mill that I have tried, the first one went so deep into my spoilboard that it broke off when it hit a screw. The first end mill was the same tool, just a down spiral instead of up. The tools don't appear to be slipping in the collet. I did notice on the tool that broke, that the pass depth was set to 1.5". I changed it on this tool to be .25". Getting back to the tool database, could I have things set improperly in there? Thanks again for all your help.
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Yabba » Thu Mar 28, 2019 10:07 pm

I just looked at my tool database, and some of the tools have pass depths that are even greater than the tool diameter... is there a guide as to what the pass depth should be in comparison to the tool's diameter?
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Rcnewcomb » Thu Mar 28, 2019 10:52 pm

is there a guide as to what the pass depth should be in comparison to the tool's diameter?

For light-duty machines the pass depth should probably be no more than 1/2 of the tool diameter, i.e. 0.125" for a 0.25" end mill.

Big industrial CNCs with 40hp spindles can cut 3X the tool diameter.
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3505
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Cutting too deep!

Postby jfederer » Fri Mar 29, 2019 3:02 am

I had a look at your file and see nothing obviously wrong. I agree with Randall though, I would use a smaller pass depth. I seldom use more than 0.125. But I don't think that's what's causing the problem.

An obvious question: have you tried running the outline path first, then the V-bit? If the depth problem then happens with the V-bit, you'll know it's not the tools database causing this. And are you saving the paths as 2 separate files, or as 1 file with a tool change? I recommend 2 separate files. I name them in such a way as to make the sequence clear on the pendant, something like 1Trivet250EM.nc, 2Trivet250V90.nc.

Unrelated, my spindle was making bearing noises so I just received a replacement under warranty. This one is much quieter, and has clean collet threads. It might be safe now to tighten the collet a bit more than what I told you earlier.
Joe Federer

www.fabrikisto.com
www.federer.ca
User avatar
jfederer
 
Posts: 33
Joined: Tue Nov 27, 2018 1:09 am
Location: Horton Township Ontario Canada
Model of CNC Machine: CanCam D23M

Re: Cutting too deep!

Postby jfederer » Fri Mar 29, 2019 3:08 am

I just thought of another possibility. A couple of days ago I changed measurement units to mm for a project, but still used the (inch) Post Processor. I had a similar problem to yours. I don't know if it was the units getting mixed up or I forgot to reset the Z, I didn't explore that further. I just switched back and everything was fine. I use the "NC Studio CC ATC Arcs (INCHES)(*.nc)" PP.
Joe Federer

www.fabrikisto.com
www.federer.ca
User avatar
jfederer
 
Posts: 33
Joined: Tue Nov 27, 2018 1:09 am
Location: Horton Township Ontario Canada
Model of CNC Machine: CanCam D23M

Re: Cutting too deep!

Postby Yabba » Fri Mar 29, 2019 7:29 pm

Thanks, I hadn't considered using separate files for each tool change, I have always done them as 1 file. As for the noise, my only issue with the machine is the fan noise... already had it replaced once - they just use crappy fans. I think I may have the problem solved... spoke with the guys from cancam and they sent me a video on zeroing out the z offset on the pendant. I'm heading to the shop now to have a look... not sure how it could have changed, but that would make sense.
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby Yabba » Fri Mar 29, 2019 11:14 pm

Well, the offsets were not the issue... they were all set to 0. I did see a couple of other things though. There were only 8 tools listed in the pendant, and I use tools numbered up to 13 - I added 5 more. After speaking with Cancam again, they told me to change the distance that the spindle rises after setting z to zero... it defaults to .389, I changed it to .1 - he recommended doing this due to the fact that my machine does not have great z travel, and with my spoilboard and material both being 11/16", there was not much room left for the spindle to rise after using the calibration tool for z. I have yet to re try the project, I'll post results.
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Re: Cutting too deep!

Postby martin54 » Sat Mar 30, 2019 1:52 am

Yabba wrote:Well, the offsets were not the issue... they were all set to 0. I did see a couple of other things though. There were only 8 tools listed in the pendant, and I use tools numbered up to 13 - I added 5 more. After speaking with Cancam again, they told me to change the distance that the spindle rises after setting z to zero... it defaults to .389, I changed it to .1 - he recommended doing this due to the fact that my machine does not have great z travel, and with my spoilboard and material both being 11/16", there was not much room left for the spindle to rise after using the calibration tool for z. I have yet to re try the project, I'll post results.


You've got loads of room for z travel, I have 55mm clearance under my gantry :lol: :lol: :lol: If the people at Cancam have told you to reduce the z axis after setting your z zero then they must think there is a possiblilty you are topping out the z axis which will cause the axis to loose steps. If that is the case then you might want to have a look at your safe z height & gap above material n the toolpath set up form, Vectric tend to set these at quite a high value by default. :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 4526
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Cutting too deep!

Postby Yabba » Sat Mar 30, 2019 4:53 pm

Thank you, Martin54. What do you think is a reasonable safe gap? I'm not concerned about stepping over clamps, etc.
Yabba
 
Posts: 13
Joined: Sat Mar 02, 2019 12:07 am
Model of CNC Machine: CanCam D23LT

Next

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 4 guests