Help -- Toolpath for grooves (slits) along length of Glass tubing in rotary axis

[adammeinke]

Hello, I've always been able to figure out processes and techniques either by trial and error or scouring the forums  but I am stuck. I honestly am not smart enough to figure this one out, nor do I know if fusion can do it, because I havent been able to find my same question and scenario asked before.

What I am trying to achieve is to cut slits lengthwise (y) on a length of approx 17mmx1.5mm pyrex tubing, and mounted in my rotary axis along the Y on my 3040 machine. The tool I am using to cut these slits is the following, a Varenkor jade slicing blade, (pn# 2113-190)

19mm x 0.45 mm:

Since the tool will be mounted upside down in the spindle, I need the tool to approach the tubing offset from the side, leaving clearance for  19mm cutting disc, then move along x to enter the "tangential" cut.. then move along y to cut the lengthwise slit, and then retreat back out of the part along x until the cutter exits the glass (10mm or more since the blade is 19mm). 

All I can get fusion to do, no matter what I do is to have any milling tool I choose or make use the bottom of the tool, when I need the side edge of the diamond blade to be the ONLY cutting contact surface. The blade needs to enter the part at a 90 degree angle, The tubing will be horizontally mounted above the bed along the Y direction in the rotary chuck and supported at the other end with the endstock swivel or whatever its called. I am hoping to create a toolpath that will bring the cutting blade adjacent to the tubing and slit lengthwise a preset distance, and then duplicate this toolpath in a circular pattern to alter the number/thickness  of slits depending on what part is being made. 

I am including a file of the model I have created. I do not know if my 'setup' preferences are correct in Manufacture.. and there are no toolpaths because I havent even been able to get close. The slits visible in the file were crudely designed so if there is a better way to CAM this (maybe just using tracing  sketchlines in a circular pattern to attach a toolpath to... I don't know. I have tried using a construction plane to keep the blade away from the part, but I honestly know I'm doing it wrong.

All things said, all I want to be able to do is create toolpaths to cut slits along the length of a piece of tubing (evenly spaced) specifically using a "cutoff wheel" type bit. The design can vary in execution as long as it creates slits. Straight Slits that begin and end before the end of the tubing. 

Thanks to any input anyone can give me on this! I've mainly been trying form mill and slot mill, using comparable dimensions to the diamond blade I want to use.

Thanks-

Adam

[matty.fuller]

You'll need to define your tool as a Slot Mill rather than an end mill, then use 2D Contour with the appropriate lead in/out to ensure it doesn't try to plunge through material. You could then probably use a Pattern to get all the slits as copies of the first.

Not sure what you mean by mounting it upside down, but it is definitely not going to work when defined as a Flat End Mill.

[adammeinke]

Thanks! Matty.fuller.  I have tried using slot and form mills already and seem to not be having luck. The tool seems to want to crash through the center of the tool. I am obviously doing something wrong. Do you or anyone have some further info as to lead in/out and/or anything else I can do to make this work? Thanks for your help

[Don_BI · Accepted solution]

You are right with slot cutter tools.  I attached your file with a tool path to view.  Obviously you will need to adjust feed and speed.  You can adjust a lot to get the ideal cut.  I just modeled at 19mm x 1mm tool but you will need to update that.

Not sure how your machine works if you have rotary calls or what so you can write a single program and just repeat it and use a macro call to rotate your part x degrees y times.

[adammeinke]

Thanks so much. I will download it now and see if we're on the right track. I am amazed at there being already two responses to my questions in under an hour! Makes the subscription worth it already. I will get back here shortly and let you know my results. Thank you! Don_BI

[adammeinke]

Jeez.. have I got a lot to learn. This is like, EXACTLY what I have been trying to do for literally months. What exactly did you change in the settings to achieve this?  Are there settings for lead-in and out or stay-down etc? I just want to be able to recreate this and understand what is happening.

I see you added a line on the inside of the groove, why does the toolpath not normally follow the groove I designed? I don't care if my design is just a pattern of lines like this.. can I do that instead of going to all the effort to design and extrude grooves?

And lastly, can this cut you've set up for me be made into a circular pattern, (ie, slit, then clear the tool from part, rotate part to next slit, and then continue on around in one operation? 

And as far as axis calls, or something like that you mentioned, I don't know? I recently changed to Uccnc so I may end up having to make these parts using Mach 3 unfortunately, since word on the street is that uccnc doesnt do Rotary axis? or it doesn't have an offset ability for it?? correct me if I'm wrong. I would much prefer uccnc.

Thank you so much for the help

[adammeinke]

I was able to recreate the toolpath, thank you again. I never noticed the little red arrow, which tells it which side of the line to follow *DOH!* no i see why the tool kept trying to be smashed down through the side of the part and be cut from the inside out. That little red arrow made all the difference! Fusion is so complex and customizable that I get into the weeds pretty frequently. Patterned file is attached, I'll try air cutting this tomorrow. Thanks again!

adam

[Don_BI]

It was most likely the red arrow messing you up,  it by default was also crashing as it was trying to go on the inside, clicking it flips the cut side and then it works.

So I just selected a inner edge(contour) and then verified the arrow was outside of the part.  Then adjusted the Tangential fragment extension distance in the passes tab to bring the cut inward on the profile.  Umm start late and end short  change it and you will see the effect.

I would write this as a single program and do a G00 A15.00 command to rotate the axis 15 degree. then G00 A30.00 and so on.  you "could" also do this in Fusion with Manual NC Command and copy and paste tool operations.

So:

G00 A0.00

Cut Program

G00 A15.00

Cut Program (Copy)

G00 A30.00

Cut Program Copy

and repeat.

I am assuming A axis is your rotary. could be B or C. 

Also G01 A15 F10 would move at 10 units per Sec/Min depending on your setup if you wanted slower rotations.  G00 is Rapid

I know this would work in Mach, I have not used  uccnc but a very fast google search makes me think you can absolutely do this with a "4th axis" rotary.  I am sure you define the axis as a rotary or angle axis.  If your controller has the axis output.  getting in the hobby stuff a lot of assumptions are made.

Also assume all lead in/out feed rates are cutting so use the same feed rates.  Since we are using the leads to plunge cut the part.

Let me know if that helps.

[Don_BI]

Congrats you figured it out as I did the reply. 😉  Let us know how it goes

[adammeinke]

Thank you again times a million! I am on west coast US and need to get in bed but first thing tomorrow I will get the two files you just posted above opened up and inspected. I never should have been so stubborn as to not ask in the forums. I'm so grateful for the help, I can barely contain it!! Thanks for the tip on the tangential extension I think it is.. I'll see if I can emulate that "late start early end" method.. Thanxxxx