Shopbot users - what have you learned?

[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 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?

[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.

[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