Multicam Router

[Bubba85]

Hello,

 

I am fairly new to mastercam. I mostly do simple 2d alum. sheet metal work on our multicam 5000 series router. However i am looking to speed up the process a little and was wondering if anyone else is doing sheet metal on a wood working router.

We are currently using Onsrud 63-000 series cutters running at around 750sfm and a .003 chip. does anyone have any suggestions??

 

Thanks in advance.

[Marshal]

Hello,

 

I am fairly new to mastercam. I mostly do simple 2d alum. sheet metal work on our multicam 5000 series router. However i am looking to speed up the process a little and was wondering if anyone else is doing sheet metal on a wood working router.

We are currently using Onsrud 63-000 series cutters running at around 750sfm and a .003 chip. does anyone have any suggestions??

 

Thanks in advance.

 

what kind of thicknesses are you doing?

 

I've tried 0.025 and 0.016" aluminum sheets in the past on our AXYZ (Pacer) router and hadn't had that good of luck, but I've found some new ways that might help, if I ever get the chance to test them.

 

The biggest problems I had with cutting the sheet aluminum on our router was keeping them held down with the vacuum, and the edge finish. Granted, we were doing some parts that a vacuum hold down isn't exactly ideal for, since they were only about 0.5" wide in most cases. However, I've recently started working with a product called "Vilmill" that looks like it'll help with the hold down quite a bit. It's basically a 0.010" thick fabric, with an adhesive on it that's activated by the heat of the cutting action. The adhesive helps with holding the parts down when they're cut through, and then it peels off without leaving any residue. I think it will help with aluminum quite a bit, but I've only used it to help with plastics so far.

 

I haven't run aluminum in quite some time so I can't really help with feeds/speeds much. I was running close to that 750sfm and 0.003 chip that you're running at now the last time I tried any aluminum. The Onsrud cutters definitely seemed to give the best results, but they still didn't meet our demanding quality requirements.

[Bubba85]

We run anywhere from .011" to .250", and most of our parts are pretty small 2"x2" roughly.

 

We have two of the for mentioned routers, one has a .750" mdf board on the bed to allows vacuum to pull through it, but I still have to add extra wholes in between the parts to screw the material down to try to eliminate chatter due to poor vacuum.

The other machine has a custom alum. vacuum plate that we use the Vilmill that you mentioned. (We have to iron it to the material before putting it on the machine, but it helps.) It seems that the edge finish varies from job to job, some turn out great as others have an extreme amount of chatter, which I blame on relying completely on the vacuum.

 

The whole reason i am researching this is our machines are becoming over scheduled, and my boss (who knows nothing of machining) on me to speed things up. Trying to explain feeds and speeds to him is like talking to a wall.

[Tyler Robertson]

Get some answers on here and maybe show him the thread afterwards - that's worked for a couple other guys I've talked to with a boss that doesn't believe someone (except maybe put tape over the parts about him)

 

all I've done with sheet has always been waterjet srry

[Marshal]

It certainly sounds to me like you've already hit that max speed. Depending on how the machine is set up, I don't imagine that your router is actually hitting that type of feed rate before it has to switch directions on the smaller parts. I know our AXYZ router takes a bit of distance to ramp up to the specified feed rate.

[Ron Branch @ 5th Axis]

Revere cut endmill to push it down verses pulls it up. On a that router you might at what I would call the ceiling and be glad you got there. I have done some pretty amazing stuff on routers, but at the end of the day they are a router not a full blown milling center. Might try some dynamic stuff to rough out slots where .25 endmill would go though using a .187 endmill then leave a .002 finish cut to clean up the edges at 4000 sfm and try the dynamic stuff at the max speeds and feeds problems is routers are great a long cuts, but the ramp up and down in feed rate needing to maximize some strategy like this might not be practical. Do some test cuts and see if you can get away with that and use it to your benefit. We were doing some high speed cutting on routers using a light depth of cut, but max rpm and max feed some years ago and getting some pretty impressive results. Really comes down to work with what you got or look to what is going to improve and help grow your company?

 

HTH

[Josh Kinney -Elite Engineering]

You want the 63-600 series. I ran these at 18-25K, 0.200" DOC and 320-400IPM with only air blast. Router Bits last days/weeks depending on the cut time.

 

I've cut literally thousands of sheets this way ranging from 0.020" to 1" thick.

 

The trick is cutting within say 0.010" of breaking through and tabbing the last pass (cutting through) with interconnecting tabs. You can use "remachine" and have MasterCam drop in and just remove the tabs....

 

Josh-

[Josh Kinney -Elite Engineering]

My experience is on MultiCam routers. I used do onsite training and support for this very thing.

 

Josh-

[Bubba85]

You want the 63-600 series. I ran these at 18-25K, 0.200" DOC and 320-400IPM with only air blast. Router Bits last days/weeks depending on the cut time.

 

I've cut literally thousands of sheets this way ranging from 0.020" to 1" thick.

 

The trick is cutting within say 0.010" of breaking through and tabbing the last pass (cutting through) with interconnecting tabs. You can use "remachine" and have MasterCam drop in and just remove the tabs....

 

Josh-

 

 

 

Thanks, I'll give this a shot. I'll post results later.

[Marshal]

You want the 63-600 series. I ran these at 18-25K, 0.200" DOC and 320-400IPM with only air blast. Router Bits last days/weeks depending on the cut time.

 

I've cut literally thousands of sheets this way ranging from 0.020" to 1" thick.

 

The trick is cutting within say 0.010" of breaking through and tabbing the last pass (cutting through) with interconnecting tabs. You can use "remachine" and have MasterCam drop in and just remove the tabs....

 

Josh-

 

what kind of fixturing do you do? Just rely on the vacuum, or do you have other methods?

 

And is it just me, or does the Onsrud website absolutely suck to find anything you want to order?

[Josh Kinney -Elite Engineering]

Crappy vacuum through Masisa (MDF). I always screw the Masisa right to the deck so it can't move around. I also generally clamp the edges and place strategic screws through the sheet along with tabs. As long as you do all the roughing passes while leaving a skin the sheet stays in place. I always go with a max DOC of 0.200".

 

There's a lot of technique involved in how/when you cut section of the sheet.

 

Yes the Onsrud sight is atrocious.

 

Josh-