What's new
What's new

Reducing Setup Times/Increasing Efficiency

Miller846

Aluminum
Joined
Oct 23, 2022
Good Morning, just curious what methods you guys are using to reduce setup times on high mix, low volume jobs for VMC’s. I’ve looked at offline tool setters, and am thinking about a base plate to try and reduce the amount of times I have to find work offsets. Currently I use renishaw probe and tool setter on the machine for finding all of my offsets but I feel like there’s definitely much more efficient methods. Thanks in advance!
 
Good Morning, just curious what methods you guys are using to reduce setup times on high mix, low volume jobs for VMC’s. I’ve looked at offline tool setters, and am thinking about a base plate to try and reduce the amount of times I have to find work offsets. Currently I use renishaw probe and tool setter on the machine for finding all of my offsets but I feel like there’s definitely much more efficient methods. Thanks in advance!
With yours being low volume high mix you definitely want to look at set up efficiency. Do you use vices? Change them a lot? Fixture plates? These are the things you want to look at. I really like the Schunk Vero-S NSE3 system, but it is costly. I would recommend tracking your set up time and find where your bottle neck is. Once Identified you can look for solutions.
 
With yours being low volume high mix you definitely want to look at set up efficiency. Do you use vices? Change them a lot? Fixture plates? These are the things you want to look at. I really like the Schunk Vero-S NSE3 system, but it is costly. I would recommend tracking your set up time and find where your bottle neck is. Once Identified you can look for solutions.
Yes currently just using two standard Kurt vices. Nothing fancy. I’m looking to invest into a more modern and streamlined system soon, just trying to figure out the best direction. I utilize a ton of soft jaws, usually have to make some special fixture plates at least once or twice a week, and the rest is just standard 3 axis vice work. I’ve looked into orange vices or some sort of carvesmart vice jaws to speed up switching vice jaws. Im also looking into offline tool setters so im not tying up the machine with setting tools.
 
Offline tool setters can definitely help, but you always run the risk of fat fingering a number while typing in the offsets if you are doing so manually. Are you using the quick release jaws? Like these https://www.snapjaws.com/
The carvesmart system is good as well. If your biggest time consumer is changing jaws then focus there first. As you eliminate bottlenecks others will take their place.
 
Currently I use renishaw probe and tool setter on the machine for finding all of my offsets but I feel like there’s definitely much more efficient methods. Thanks in advance!
I think you're on the right track.
I'd also look into modular work holding, a subplate with keyways and threaded holes at specific locations, keyed fixtures and vises, and keeping at least the basic cutting tools in the ATC at all times.
 
Key your jaws to your vise body. If the vises are removed regularly [for good reason] pin them to the table.
I keep notes right in the program. (L vise L stop R vise r stop .75 par]
I use local offsets, G52 for instance.
I can go from running one type of part to another different part in a few minutes. First part is almost always a good part, requiring a few thousandths adjustment to the G52 which is itself a subroutine in the program, such that changing the one line changes the offset for all the operations in the program
Use the same core of tools. I can think of little reason to have a 1/2 5/8 and 3/4 end mill. Learn to love interpolation. The time you save optimizing that tool path is wasted if you have to change one tool. If you have for instance a lot of different sized tapped holes, keep the most commonly used ones in the tool carousel, then have several locations that are all 'temp' locations

The Blum on the Brother is pretty fast to set new tools.
 
All good advice, I currently keep all my common tools in a designated tool number that also correlates with my cam tool library. I use interpolation/boring cycles wherever I can. I guess my best and cheapest place to start is to implement some sort of quick jaw change system. I very rarely pull my vices off, I try to avoid it whenever I can. But I am always swapping between hard jaws and soft jaws so a carvesmart type system would be a big time saver. Also standardizing my work offsets I think would help quite a bit as well. I’m also looking into different cam softwares. I’m currently using fusion because it’s cheap and what I started on, it usually works just fine but the past year I’ve been doing much more 3d surfacing and fusion leaves a lot to be desired in that arena. I end up fighting the software for a an hour or two to get it to not create an extremely inefficient/choppy tool path. Also curious everyone’s thoughts on a good cam system, thanks!
 
In Fusion, I would be much faster set ups if you create a parametrically driven vise and stock. Simulate your vise, have a WCS (Bore Hole and top of bed) on the vise, use another WCS for stock. The probe is driven from the Vise WCS. Removes hand jogging the probe. Vise and stock automatically change with each part just by adjusting stock dimensions.

takes time to initially create but once you do, it saves so much time every time you set stock.
 
I’d personally throw CarvesSmart Master Jaws in your Kurt’s and call that a day. If you’re doing low volume, high mix work they are perfect for that.

Spend some time learning how to drive the 3D toolpaths within Fusion. There hasn’t been a surface I haven’t been able to handle cleanly and efficiently in Fusion, especially on a 3-Axis mill. Tons of options in there and a lot of ways to drive them.

Offline tool setters are not going to make your setups any faster, and unless you’re pushing the data automatically, you run the risk of inputting data incorrectly and slamming your machine. Get proficient with the built in cycles on your machine if there are any. Many posts in Fusion will even output the option to touch off tools at the beginning of a program so the program will handle touching them off at the beginning of a cycle then you just toggle it off for the remainder of the run.spindle probe can find your WCS on its own if your CAM is setup correctly.

Standardize your tool library, model your table and workholding and build templates within Fusion to simply drop your part file in and regenerate the bulk of the toolpaths and add what’s needed. Over time you’ll build enough templates to handle most parts without much editing/adding of toolpaths. Let the CAM, spindle probe and tool setter do the work.
 
The probe is driven from the Vise WCS. Removes hand jogging the probe. Vise and stock automatically change with each part just by adjusting stock dimensions.
I do something along these lines, but in the form of an aliased macro, which sets my new work coordinate system. Example is the left edge of my vise jaw, and top step of my jaws, is G54.1 P40. In the macro address line there are 3 variables for which vise, which step, and which offset I'm wanting to adjust (G54). Then the next three variables are distance from G54.1 P40 in X Y Z for my new G54 work offset. After I run my aliased G-Code, I run a quick probing cycle to find the true location of my part. I have all of the Renishaw probing routines saved in a text file so I can just copy and paste into the posted code. It takes me about 20 seconds of hand editing to be able to run it. In the future I hope I can get the probe package in my CAM and edit my post to output my macro line.

I hate hand jogging my machines. Especially if I'm hand jogging to a location to probe a location. With this macro I haven't hand jogged to set a work offset in over 3 years, and it's been great. It's a lot quicker as well, so it's a two-stones one-bird, solution.
 
I do something along these lines, but in the form of an aliased macro, which sets my new work coordinate system. Example is the left edge of my vise jaw, and top step of my jaws, is G54.1 P40. In the macro address line there are 3 variables for which vise, which step, and which offset I'm wanting to adjust (G54). Then the next three variables are distance from G54.1 P40 in X Y Z for my new G54 work offset. After I run my aliased G-Code, I run a quick probing cycle to find the true location of my part.

Exactly this!

I'm happy to share my macro to do this. However it's for a Speedio (Fanuc alike G-code controller).

I insert the call as a "manual NC" line at the top of my Fusion setup. It may sound terrible but you can measure your XYZ in CAD and generally you only have 2-3 options (you need one per type of jaws you use). So I just have them as templates with names (8" serrated jaws left side) etc.

I've nothing against programming against the zero point, but I prefer to have my WCS on the part (yeah, million ways to slice this...). The probe is excellent for refining the estimated and my goal is to do no WCS setup on the machine itself.

For short run parts I probe the location every part (so nothing to forget. Just run the one up). For longer runs I will split up the program into a "setup step" and then the main program without probing (or perhaps probe only X or whatever).
 








 
Back
Top