X5 Optirough video

[Redfire427]

Hey guys,

 

Like most of you, I am becoming more and more familiar with the new features in X5. One new feature is the Optirough toolpath which is a very efficient new machining strategy designed specifically for high-speed machining. As our company specializes in this field, I thought I would make a short video demonstrating the powerful approach this toolpath offers. I know many of you do not have access to high-speed equipment, but this video should show what a powerful combination this toolpath used on the right equipment can deliver.

 

The machining centre is a Makino S56 3-axis vertical 13K spindle with a cat40 taper. This is a wicked fast machine with 1600ipm feedrate capability.

 

This workpiece is a core for a plastic injection mold producing a cap for a shampoo bottle. The material is stainless 420. I used a variable flute 5/8" bullnose 4-flute solid carbide endmill. The stategy used is as follows:

 

3500 rpm

125 ipm feedrate

.625 depth of cut

.050" stepover

.050 step-up

Rapid feedrate 700 ipm

 

 

The run-time from start to finish on this core was just a tick over 10 minutes. This endmill lasted for all 18 cores.

 

The purpose of this thread is to show others the hard work CNC Software put into this new strategy and show it being used in a real-world situation. Well done CNC Software.

 

Enjoy.

 

Carmen

 

 

[Newbeeee™]

Thanks Carmen, Neat video.

I think we'll have a look at upgrading to X5 over xmas.

Cheers

[Chris Rizzo]

Hey if you don't mind feel free to enter your parameters into the dynamic mill database. Links are in my sig.

[TK-32™]

cool video!!!

[ATG]

How much time do you think you saved? It would apear to be allot....Nice video

[MotorCityMinion]

Here's the kicker .. look how far out of the holder the tool hanging. 

[Goldorak]

prosin , try this next time

 

get a smaller tool lile a .500 or .375 , they are cheaper and faster due ro rhe faster rpm so you get faster feedrate and less stress on the machine, and your machine can go a lot faster than that

 

BTW very nice video !

[Redfire427]

Let me respond to some of the comments.

 

Chris Rizzo: I will enter my data.

 

TK-421: Thank-you

 

ATG: It is hard to say how much time we save with this approach as we do not do production. What I will say is that the tooling cost is almost zero. What I mean is, this endmill was in the $80 range and it lasted for all the cores. I can still send it out to have the flutes cleaned-up and use it on another job. By comparison, if I were to use a inserted flycutter, the insert cost and the added toolpath run-time would be much, much more. This toolpath runs very smoothly on our machines. It may sound a little harsh in the video, however, it isn't.

 

MotorCityMinion: The tool stick-out is only .050" more than the longest projection of the part. In this case, the stick-out was 2.3" What you did not see in the video was the final depth passes as it made the video too long for Youtube to accept. It also performed a helix-bore in the centre of the oval.

 

Goldorak: My original plans were to use a 1/2" endmill for this job as the speed of the machine is truly impressive. The reason I didn't is because my local supplier didn't have any in stock so 5/8" was the next best choice. I think the machining time would have been comparable though, because I would reduce the width of cut to .035" but increase the feedrate to 200ipm, so the metal removal rate would have been roughly the same. You are absolutely correct in your comments, and for video purposes, I wish I had ordered the tool sooner to have on hand for this video. What is truly mind-blowing on this particular machine is when we rough pockets/cavities at 400 ipm with a 3/4" feedmill. I never grow tired of watching this even after 7 years of doing this type of work every day.

[Bob W.]

Great video. Thanks for sharing!

[MrFish]

Have you optioned the cutter to stay down on re-positions or is that the way that the toolpath works, seems that on a slower machine that can't rapid as quick in a contoured motion that the toolpath might be a bit slow unless you could retract Z to reposition in a straigh line format?

[Redfire427]

Have you optioned the cutter to stay down on re-positions or is that the way that the toolpath works, seems that on a slower machine that can't rapid as quick in a contoured motion that the toolpath might be a bit slow unless you could retract Z to reposition in a straigh line format?

 

I have it set using the micro-lifts function so the tool retracts .002" in "Z" between cuts and "rapids" to the next cut where it then ramps back down to the correct z-value. There is a way to adjust the toolpath to do what you are asking, however, as we only have high speed machines, I have no need to educate myself to do as you asked about.

[MrFish]

I have it set using the micro-lifts function so the tool retracts .002" in "Z" between cuts and "rapids" to the next cut where it then ramps back down to the correct z-value. There is a way to adjust the toolpath to do what you are asking, however, as we only have high speed machines, I have no need to educate myself to do as you asked about.

 

 

Good to know, don't have X5 yet as it hasn't been delivered in NZ. Think our DMG will probably handle the same strategy as you are using but doubt the HAAS machines will. Looking forward to doing some testing, X5 looks to have some nice new features.

[Redfire427]

Good to know, don't have X5 yet as it hasn't been delivered in NZ. Think our DMG will probably handle the same strategy as you are using but doubt the HAAS machines will. Looking forward to doing some testing, X5 looks to have some nice new features.

 

If you are a maintenance customer, you can just download X5. Your DMG will haul the mail with this toolpath. The Haas's might not be too bad either.

[Bob W.]

With a Haas it is very dependent on the machine's accuracy setting. This can be controlled in the G code with G187 P1 (rough), P2 (medium - default), or P3 (finish). I control these in my post with misc integers and for roughing adding G187 P1 right after the tool change will have the machine running twice as fast, literally. You need to watch out though because if you don't leave enough stock it WILL clip corners. I usually leave .015" to be safe. To reset to default simply add another G187 before the next op. I believe the Haas setting this alters is either 85 or 191 and it reverts to default with either another G187,an M30, or hitting the reset button.

[David Conigliaro CNC Software Inc.]

Those micro lift reposition moves can optionally be output as traditional retracts if you wish. There are retract controls on the cut parameter page. This toolpath runs very well on a HAAS or similar machine. We tested it on a variety of machines, Makino S56, Makino V33i, old OKK, Okuma VMC, various HAAS models including the DT1 ranging from older late 90's models to 2010's, etc...Its for all CNC machines, no matter what the capabilities.

[The_Evil_Machinist]

.Its for all CNC machines, no matter what the capabilities.

 

That's an understatement. I use it while drip feeding to my 91 akira seiki v5 and it still runs great.

[Mcam Nut]

Thanks for the video, that endmill worked great considering the distance it was hanging out. Great job