Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Setting up Slitting Saw

14 REPLIES 14
SOLVED
Reply
Message 1 of 15
jeph_s22
355 Views, 14 Replies

Setting up Slitting Saw

Hello everyone.

First time using a slitting saw - can anyone help me out with setting this one up? I was thinking 0.125" doc on this one. Part attached.

Any help is appreciated.

14 REPLIES 14
Message 2 of 15

I made a few tests for you, attached for review.

Message 3 of 15
seth.madore
in reply to: jeph_s22

It depends, I suppose. What is the tool material and what is the material being cut? Do you have a stout machine, or do you need to baby it thru the cut?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 15
jeph_s22
in reply to: seth.madore

Hi Seth,

Material being cut is 1045 and 1018 mild steel. Tool material is HSS. Machine is a Mori Sieki NL3000y, so enough machine for the job i would say.

Message 5 of 15
seth.madore
in reply to: jeph_s22

Yeah, the Mori is a stout machine. Personally, I would make an attempt at doing it in one shot (provided you've got a couple extra saws (just in case)

Also, if you're in the USA, both Harvey and Internal Tool make some carbide slitting saws in smaller diameters, you wouldn't need to go with a 4" HSS saw...


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 6 of 15
jeph_s22
in reply to: seth.madore

I only got the one 4" HSS saw for this job. So taking it easy this time would probably be the way to go.

 

Message 7 of 15
seth.madore
in reply to: jeph_s22

Hmm. I'm never comfortable going into a job with only one tool at my disposal, but it's also easy for me to say as you're likely not the one making that judgement call.

 

I'd certainly reduce your feedrate. .001" per tooth is going to be quite aggressive. As an example, I run a 1.5" (12 teeth) saw in stainless at 600 RPM and 2.0 IPM. You're running at 57rpm and 2.0" IPM. I'd likely bump the speed up to 75sfpm and reduce the feed per tooth by about half. Depth of cut (in 3 passes) would be .150 per (although I think you could do this in one shot, just taking it slow and plenty of coolant)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 8 of 15
programming2C78B
in reply to: jeph_s22

ours has more like 100teeth so we do .0001 cpt, 3x thickness as DOC, and about 50-75sfm in stainless. Everything works out on size. There are some great guide PDF's online if you just look into them. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 9 of 15
jeph_s22
in reply to: seth.madore

@seth.madoreI do buy my own tools but was unsure what will work best for me so I just got one unit to try for a quick job. Are your saws carbide or hss?

I will try with the suggested feeds and speeds, thanks for your input on this.

@programming2C78BI actually did try looking up online but couldn't find much.

Message 10 of 15
seth.madore
in reply to: jeph_s22

Carbide, always carbide 🙂

 

(that's not entirely true, there are times when I have to use a gigantic milling arbor and .50" wide x 4" dia HSS saw)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 15
jeph_s22
in reply to: seth.madore

at 0.0005 ipr and 75 sfm Fusion estimates a 3" cut, 4 passes to take 20 minutes. Does that sound accurate to you? sound like a long time.
Message 12 of 15
seth.madore
in reply to: jeph_s22

It's not .0005 ipr, but IPT (inches per tooth). It should be about a 12 min cycle

(which is also why I would prefer carbide and a single pass)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 13 of 15
jeph_s22
in reply to: seth.madore

Hi Seth,

I got the following error log when I try and output this code; can you tell me what this means?

Screenshot (3).png

Message 14 of 15
jeph_s22
in reply to: jeph_s22

Part again attached.

Message 15 of 15
CNC_Lee
in reply to: jeph_s22

@jeph_s22 

 The toolpath could be out of the machine travel linits as defined in the machine configuration. It is a bit haed to tell without the post processor.
 

If my post answers your question, please use Accept as Solution.

CNC Lee
Fusion 360 CAM Post Processor Expert
https://linktr.ee/cnclee

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums