trying to make tool path from a solid curved stock

[jimbocurtis]

I am trying to CNC a wooden mandolin neck from a nice 3D drawing I have.  My stock is not a solid block of wood, as the setup page thinks it is.  so I chose to mill it from a solid and no matter which roughing strategy I use, adaptive or pocket 3d, each one creates excessive passes with the bit in the "air".  my stock is very close to what my model looks like.  I have posted 3 screen shots here, one of the model, one of each of the milling strategies.  If I were using a solid block of wood- it would be great.  but I am not and it's creating a lengthy cut time.  any ideas of how I could get the tool path to start and stay much closer to the model?   thanks for your help, anyone that has a suggestion.  I have thought I might need to draw bounding lines on the model.  I am not sure if that would solve it, or how to even do that...  again, thanks for any and all suggestions!

[randyT9V9C]

Export your model and upload it.

Create a roughing operation that leaves the material close to your rough band sawed shape. Then use rest machining for your following operations. Once you've generated all the paths only post the paths that you actually need.

Another method would be to insert some construction plans with boundary sketches allowing you to select the boundary and levels for each region.

[Laurens-3DTechDraw]

Use rest machining.

And turn form job stock on.

[randyT9V9C]

I tried Laurens' method. It works well. In the model I created a sketch and extruded it to form a body. On the Setup tab I selected the neck as the Model body. On the Stock tab I selected the rough stock body I created. On the operation Geometry tab I enable Rest Machining and set the Source to From Setup Stock. I attached my model using a guitar neck I found.

Lauren, where is the setting "form job stock on"?

[Laurens-3DTechDraw]

Sorry.

In HSMWorks a setup is called a job.

So you did the right thing. I just used the wrong name for the same thing.

[jimbocurtis]

Wow, you guys are great, and smart! I will go to my shop today and try
this. But now, if I may ask you this: would a rough pass with a flat end
mill be necessary or could I go straight to using a ball end mill? Both are
half inch. And what type of tool path would you use? Thanks again, y'all
have been so helpful!

[randyT9V9C]

I'd imagine if your removed the bulk of material with the bandsaw you may be able to go straight to a ball mill, especially if the ball mill is designed for wood carving. I'm not a wood worker so YMMV. 

A quick, random, google search found these ball tools:

https://www.vortextool.com/index.cfm?fuseaction=category.display&category_id=23&CFID=31113149&CFTOKE...

[jimbocurtis]

thanks for your input - very helpful.  I was able to make a tool path that looks good, but something strange happened.  the tool did not move at all like the tool path showed.  I thought maybe it was because there was not enough Z clearance for the retract, so I re-ran it with a short bit with plenty of Z clearance and it still misbehaved.  I have never seen this happen.  any ideas of what to do if the bit is deviating from the tool path animation?  

[jimbocurtis]

thanks, that's what I thought, except it will not really mill my low flat side areas of the model.  I have a pair of ball and flat bits, but they are too long.  I might have to cut them down.... fun!

[randyT9V9C]

Verify your WVS is correct. I back plotted my path and they appear correct. If it still doesn't appear correct export your model and post it. What post processor are you using?

If you want to finish the bottom edge of the part with the ball mill, simply define your part bottom on the Heights tab to a value below the part, at least equal to the radius of your cutter.

[jimbocurtis]

I discovered that it was the safe height limit in my CNC controller that needed to be changed. Seems like there is always something! Thanks for your suggestion to use the lower clearance for the round bit. Great idea! You folks really are smart and I appreciate your help!

[jimbocurtis]

I ran the file after fixing my Z-height limitation and watched in awe as it milled it completely wrong in nearly every way.  I aborted the process when it was clearly cutting into an area that was meant to be left alone.  I cleaned everything up, took the tool out and the workpiece off and turn the machine off.  I have spent nearly a week trying to get this cut and I feel pretty defeated.  If anyone wants to see my file, the tool path used and the thing it cut, I'd be glad to send it.  But at this point, I may just walk away from this.  It's taking way more time than it's worth.   thanks for all your input, it really helped me get along to where I thought I was needing to go!

[randyT9V9C]

Jim, it is likely something fairly easy to fix. I know your frustrated but I'm certain it can be sorted out. Hopefully you didn't scrap your fine material. 😉

Export your model (click File, Export) and attach it so we can see what's going on. Also, attach your g-code file that you attempted to run. 

Also, what machine are you running and what post processor are you using?

[jimbocurtis]

oh you are too nice!  no, I didn't scrap it, it's so much work involved, I figured I'd just walk away for awhile and work in the analog world for awhile.  

I have attached the model and a photo of what I got, despite the tool path looking great on the computer.   I am using an Axiom AR6 Pro with industrial controller and the G-code was created specifically for it by Silverhawk, since Axiom didn't give Autodesk the machine codes to make a post for their machine.  I mill other things, such as arched 3D plates for instrument tops/backs.  I have never had anything like this occur.  not sure what to do, really.  Maybe if you have a moment you can take a look at my files and see what you think.  thanks so much for your kind and generous time!

[randyT9V9C]

Looking at your pictures, did your stock move and/or steppers lose some steps? After you stopped did you return the machine to your origin point to verify it hadn't moved or shifted?

I back plotted the path that I posted from your model. It looks fine. Post your g-code file and I'll back plot it for comparison.

[jimbocurtis]

I did not move it back home until later, after I had turned the machine off, someone else asked me if I had done that because they asked if the stepper motor skipped.  I did not hear it skip, I watched it for 10 minutes during the while.  it seems like it was moving inward and downward, as the Z level changed and the side profile of the neck was way chopped in and the bit went thru the fingerboard and all the while the neck heel stayed OK.  so it is really confusing me.  I will attach the code now.  thanks again for your help!  actually now I just tried to attach the g-code file and it won't let me.  the error says:  

• The file flat4.mmg does not have a valid extension for an attachment and has been removed. 3dp,3ds,ach,ai,art,ass,asx,avi,axm,bm,bmp,cfz,chm,cps,csv,dbf,dcl,doc,docx,dst,dwf,dwfx,dwg,dws,dwt,dxf,dyf,dyn,eco,env,eps,esri,f3d,f3z,fbx,fm,gif,gz,gzip,iam,ics,ide,idw,iks,ipn,ipt,jfif,jpe,jpeg,jpg,log,lsp,mac,max,mb,mp4,mpg,msg,nc,nc1,nwc,nwd,nwf,obj,obk,pat,pc3,pdf,pkt,png,png,ppt,pptx,prj,psd,rar,rfa,rft,rlf,rtd,rvt,sat,sdf,sdf,sdf2,sdf3,shp,shx,simstudio,sldasm,slddrw,sldprt,sol,spf,step,stl,stm,stp,svf,svg,text,tif,tiff,txt,vcf,vtf,vtfx,wmv,xls,xlsx,xml,xps,zip are the valid extensions.

[randyT9V9C]

Change the extension from .mmg to .txt. Or put it in a zip file.

[jimbocurtis]

ok here it is

[randyT9V9C]

It back plotted fine. I don't see any rapids through the stock. Nothing obvious. Based on the photos and the back plots I'm suspecting material shift or lost steps. Being that you've been routing other stuff just fine. Try milling it out of something like styrofoam and see how it goes. Remember a long endmill can put a lot more pressure on your axis than a short one.

[jimbocurtis]

So would you recommend adjusting somehow to make up for the long bit?