Shopbot users - what have you learned?

[aphelps231]

We have a shopbot in our shop that is intended for use on wood, but I've met multiple teams who use similar shopbot routers to cut aluminum. We've tried to get it working before but we ended up breaking bits and having a hard time holding the material down to the bed.

So what tips do you have for someone who is trying to get their shopbot to cut aluminum?

[AriMindell]

We tried to use a shopbot to cut 1/4" aluminum parts for our climber.
We were actually able to cut it relatively easily with the right bit and feed speeds.
To keep the aluminum fastened down, we predrilled holes in the corners of the aluminum, and woodscrewed it into the bed.
We used the following settings and parts:
a 1/4" carbide flat end mill
10000 RPM
I am unsure of the feed speed we used, but you can figure it out for yourself with this chart:
http://www.bing.com/images/search?q=shopbot+feeds+and+speeds+1%2f4+aluminum+4 +flute&view=detailv2&&id=3D8A69C7291F45AFC372C16BE 10018AA4B57C699&selectedIndex=1&ccid=3ti9%2fpTu&si mid=608004427611244244&thid=OIP.Mded8bdfe94eed06b1 8605e2446230e1fo0&ajaxhist=0
The main problem we ran into was chiploading. We had to pause our machine every so often and remove all of the aluminum chips from the bit, or the bit would start melting instead of cutting, creating rough edges and eventually halting the machine. To remedy this, you might try a slim pass depth.

[Steven Smith]

Could you give a little more information on what you are currently doing? What bits, what is your hold-down strategy, coolant/chipclearing, what thickness and grade of aluminum, etc.

We struggled for a while to get our gantry mill to cut aluminum properly. We're currently running a 3/16" Amana single flute bit at ~50IPM and 12000 RPM (need a true spindle to run lower with power, not a router). We have a high pressure air blast that is sufficient when cutting 6061 (easiest to cut IMO) and we use a little WD40 (need to convert to a better fluid) when cutting 5052, which we use for bent parts. We can do ~0.0625 on our DOC without major issues.

We lay out our entire stock and pieces in our CAM software, and then pre-mark drilling patterns between the parts. We use wood screws on the edge to hold down the piece, then have the gantry drill its own holes in the middle of, and around every piece we are cutting out. In a ~2'x2' work area, we might end up using 20-30 screws. If you don't have your workpiece held down really well, it will vibrate against your cutter though, creating heat. A better way might be a vacuum table... but hey... we have freshmen.

One last note, you need to make sure your sacrificial bed is well leveled (flat in the Z). If you have wildly varying DOC issues due to an unlevel bed, that can eat a bit up in a hurry.

[marshall]

ShopBot Tools is actually local to us and a sponsor. We love them!

Buy good bits. We use Onsrud typically and they have a chip load calculator spreadsheet thing that comes in the back of their catalogs that is awesome.

The other big thing is to hold down your work as much as possible. There are a few ways to do it:

• Screws in strategic locations... be wary of hitting them or bits go boom.
• Elmers glue... rub it on the aluminum sheet and also on a sheet of MDF. Let it dry for a few, and then stick them together. To remove, use paint thinner or mineral oil. A bit messy but parts come out great.
• 3M spray adhesive and it's basically the same as above.
• Vacuum table but not the best for aluminum (can still slide) and I'd still use one of the other methods above in conjunction with it.

Edit: Also, if you want real tips then post your questions on their forums or call them. Both are amazing and you'll get responses.

[JesseK]

We use End Mill clamps (not sure what they're actually called) and solid steel bar (1"x12"x3") to hold our pieces down. Though our CNC isn't a ShopBot, and is 4'x4'.

[Steven Smith]

Originally Posted by JesseK

We use End Mill clamps (not sure what they're actually called) and solid steel bar (1"x12"x3") to hold our pieces down. Though our CNC isn't a ShopBot, and is 4'x4'.

Any chance you could post a picture?

I'm also interested (sorry OP! but hope it is relevant) on any fixturing people may use on a gantry mill to hold aluminum extrusion for lightening hole milling. I have a few ideas in my head, but I'd like to get it running this offseason. So far, have only messed with 0.0625 to 0.125" sheet.

[Eric Scheuing]

Originally Posted by marshall

The other big thing is to hold down your work as much as possible. There are a few ways to do it:...

We were told that double sided carpet tape works pretty well. We have yet to try, but I can't see why it wouldn't work. That stuff can be strong!

[Forhire]

We used a Shopbot this season for a lot of our parts. We also have two other cnc mills but the router has the largest area and the fastest spindle. It does 0.0625" and 0.125" sheet aluminum just dandy. Most of what we use is 5052 and 6061. Both machine similar. We also did the outer side plates from 3/8" 6061. We screwed most everything down but also hot glued a few small items.

The most important number you need is chip load (IPT). With a 1/4" cutter we nearly always use 0.002" IPT. We may have been able to go heavier but this worked consistently for us and I felt is was conservative. We used 3 flute coated endmills. If you go too heavy it may chatter or even miss steps... it you go too light it well generate too much heat and gum up. A healthy chip stays firm and takes the heat with it.

Early in the season we used WD-40. I am not a fan! Doesn't work very well and it's messy. It can smoke and cause general operator irritation. The parts would often be too hot to touch. So then we experimented with denatured alcohol in a spray bottle. This worked well. The parts stayed cool with no cleanup... but the spray bottle was wasteful. I was worried about swelling the waste board with a water based coolant. So I finally brought my fogbuster down and misted with denatured alcohol. It was a winner. We used less than a quart all season. With the misting we did 1.5xdiameter slotting in the 3/8" material. The key was proper chip load.

I just pulled up the CAM and verified the path we used. Helix in at 3 degrees, full depth 0.40", 25% step over, 0.002 IPT, 18,000 RPM, 108 IPM.



On the Centroid CNC knee mill we use a Trico MD-1200 MICRO-DROP mister with the synthetic oil. Works well as an alternative to the fogbuster. We mill steel parts on that machine.

Here's a video of the Shopbot milling thin aluminum.
https://www.youtube.com/watch?v=rFwFvM0ozno

[DonRotolo]

Randy, are you saying you cut at 0.40" depth at 108 IPM with your shopbot?

[asid61]

Originally Posted by DonRotolo

Randy, are you saying you cut at 0.40" depth at 108 IPM with your shopbot?

I googled 16 gauge (from the video) and it said 0.0625", which sounds even more crazy. That's miles ahead of all of the other routers that people list here.

How do you place your screws so that the shopbot doesn't hit them?

[Steven Smith]

How do you place your screws so that the shopbot doesn't hit them?

For us, we lay out the parts with Cut2D, which although simplistic, is fine for most of our 2.5D parts. We model the entire material piece (~2'x4') usually in CAM, and then have the mill drill its own screw down holes by placing circles throughout the material, with a diameter larger than the screw head.

We screw it down liberally.

When we add a part to the layout to cut, we'll add more screw holes around (or within) the part to ensure good hold down. As long as we don't run a cut line through our hole, we are fine. We have also learned that the bit will cut a screw

[Forhire]

Originally Posted by DonRotolo

Randy, are you saying you cut at 0.40" depth at 108 IPM with your shopbot?

Yes. We found we had better chip evacuation with a through material cut, full depth. Slotting can be problematic for sure. Endmills are designed to cut on the flutes as well as the ends. It's a lot easier to push a full length chip out of slot than a small chip from the bottom. The long chip is your friend in this case, it carries the heat and is less likely to load up. The 1.5xdiameter was pushing our luck for sure but all I had with me was some 1/4" endmills. We made 4 of these side plates... we didn't start crazy fast from the go... but by the fourth we had the recipe perfected. Our Shopbot is a PRSAlpha Buddy with the 18k rpm 2.2HP spindle.

It's possible that some of the rest of the post may be a bit off topic but the OP wanted to know what we've learned having run a shopbot. Here you go.

Understand that despite the Shopbot performing so well we had terrible difficulties with the software crashing. Little jobs that should have taken 15 minutes stretched into an hour due to lockup/pausing problems. Multiple parts and or multi-operation jobs were delayed due to lockups between parts. During the build season isn't the time to diagnose issues... we just needed it to work. We lived with it. The student that ran this machine would get so frustrated he'd leave. Near the end of the season we discovered that if we closed the RPM pane the machine wouldn't lock up as much. A little too late. This is an on top of it being a terrible user interface and using OpenSBP. Claiming to support g-code but really only handing the basic linear and arc commands. No canned drilling ops. No spindle speed control from within g-code. The list went on and on.

After the season we converted the Shopbot to use a Dynamotion Kflop motion controller with KmotionCNC. We only ran it for a few weeks before the end of the school year but it was 100% worth the upgrade. No crashes and the interface is more similar to the Centroid and Fanuc based cnc machines the students also run in the shop. Being that the students have to know some basic g-code for the other machines... standardizing makes it much easier. The shopbot was an odd duck in the shop. Here's some more information:
http://www.cnczone.com/forums/dynomo...-software.html

The adapter board that plugs in where the Shopbot control plugged in. It was designed in Eagle and sent out have the PCB made. This allowed the machine to be changed over without any permanent modifications. It includes a TTL_RS485 module that allows spindle control via Modbus directly from the Kflop. Once it came back the adapter was installed along with the Kflop. Programming is done in C so between a mentor and some students it was running in a few days. Now we can change spindle speed while running. And when we pause the work... it pauses instantly. And if there is something we don't like... we can readily change it.

Here's some photos:





Here's some UHMW being done for the first time after converting:
https://www.youtube.com/watch?v=hTLwlvJWWCk

[Forhire]

Originally Posted by asid61

I googled 16 gauge (from the video) and it said 0.0625", which sounds even more crazy. That's miles ahead of all of the other routers that people list here.

How do you place your screws so that the shopbot doesn't hit them?

It does that 0.0625 aluminum sheet so easily. The video doesn't really do it justice.

This part was done in two operations. The first we drilled all the holes while the material was clamped to the table. This included all the holes you see plus all the helical start locations in the pockets. This aided the pocket starts. We then screwed down the part through all the holes and removed the clamps. We then ran the second operation. The part takes about 30 minutes.

A hardened screw will eat and endmill in a hurry unless you just graze it. Softer wood screws can be machined right through but they require a pilot hole as they tend to tear out of the mdf.

Not hitting screws requires diligence on the part of the designers and those setting up the machines. Last year we had real issues with some parts. This season we had a student in the shop sit down with the designer prior to making the part to ensure it was machinable. This included everything from sufficient hold down locations to proper fillets and realistic tolerances. We also had the designers come in and help on a few parts. This greatly improved the workflow and resulted in parts that fit the first time.

At present we are using Solidworks and HSM Works for the cam. This was the first year we had students setting up the cam paths aside from the stuff they did using the conversational (Intercon) on the Centroid. The key is to setup a set of procedures and use them consistently.

In the fall we are planning on making a foot to hold down sheet material. Shopbot offers a simplistic version but we'd prefer to build our own. Projects teach skills. Is anyone using a foot on their router?

[kaliken]

What we founds with hsmworks is that if you make a separate assembly with your part(s) you can easily model in screws and other machine fixtures. From there you can run a model simulation with stock removal and collision detection to see if you hit any screws. If course you should always double check it.

Sent from my XT1254 using Tapatalk

[AdamHeard]

Originally Posted by asid61

I googled 16 gauge (from the video) and it said 0.0625", which sounds even more crazy. That's miles ahead of all of the other routers that people list here.

How do you place your screws so that the shopbot doesn't hit them?

Using onsrud single flute cutters and a decent machine those numbers are very achievable in .0625 Aluminun.