High Speed Machining Toolpaths on a Benchtop

[jid2]

As my conversion project slowly gets closer to throwing chips I'm starting to learn my way around some CAM packages. Right now I'm playing with HSMWorks and SolidCam, both of which are Solidworks integrated platforms. Both of these programs as well as all the other major CAM players leverage modern "high speed machining" toolpaths which look to constantly load the tool. They avoid the rapid velocity/accel changes, and width of cut increases found in tight corners or stepover areas of traditional toolpaths. They also look to used 1x to 2x the tool diameter for Depth of Cut, with less radial engagement.

Anyway - this works great on the real VMC's, but what does it mean for us garage guys with our Modded RF45's and such. Have any of you guys played around with these types of tool paths? I feel like the logic is very sound that constant loading of the tool can only be better for it. I plan on running some tests once I'm up and running.

Any thoughts or experience with this?

[mmprestine]

I have been using HSMexpress for about the last 4 months and find it to be great, other than it being free the integration to solid works was a huge draw for me. I fumbled around with CAMbam for the first year and it is good but in my opinion there is no comparison to HSMexpress. It takes a little to get configured the way you may like it but the operations are pretty straight forward. Biggest issues I had were to define origins, tops, and bottoms for the work piece but after that easy peasy. You can change all the specifics of the machining step over, depth of cut, speed, etc. to fit your machine. Not being a "real machinist" I cannot truly compare but it works very well for me and I have an X3. The HSMexpress support forum here is pretty dismal so maybe there are not that many people using it. Let me know if you need any help.
Matt

[jid2]

So are you using 2D adaptive clearing with larger depth of cuts?

The support forum on the actual HSMWorks site is very good. All of the value add resalers post there and are good at helping the userbase. If things get running smoothly on my home machine work will likely buy a machine along with the full HSMWorks package.

How is the included Mach 2 post?

[mmprestine]

Yes I am using adaptive clearing but larger depths of cuts are relative to the machine capabilities so yours will be different as they will be with a real VMC. One thing to note is that the adaptive clearing makes huge files and many cnc controllers choke with it.

I was actually referring to the support forum on cnczone, the real HSMworks one is very good.

Using LinuxCNC so I cannot answer about the Mach3 post but I would assume it to be ok.

[Flenser]

After playing around with parts for work over the last year or two, I have to say that generating stock of the correct size for a given part consumes the vast majority of machining time and causes the greatest wear on tooling. For me, that almost always involves cutting a block first on the band saw, then on the mill to a specific and (usually) rectangular dimension.

Frankly, the wizards in Mach3 for doing this suck. I would cut the stock manually before using Mach wizards. I am familiar with Visual Mill and less so with Bob Cad. Neither do this one essential operation adequately.

I wrote a couple of programs that generate this code for my particular mill. To cut stock I use cheap Chinese HSS roughers from shars. I run up to the the max flute depth of the end mill at SLOW speeds and 50% radial step overs. Mach lets me tweak the speed on the fly, and the sound of the cut is pretty informative. Generally, by the second pass I believe I have the optimal speed I can get by ear.

I dunno about cutting the part itself. Honestly, I get emotional about getting the right dimensions on the first try, even if I had to wait for an hour on something I could have cut manually in ten minutes.

[691175002]

There is no inherent reason why a lighter machine could not use a HSM toolpath. In fact, a HSM toolpath should apply less stress to the machine (thats the entire point of constant engagement).

The only potential problem is that some controllers don't deal very well massive numbers of very small movements at high speed. Calculating a constant velocity toolpath at hundreds of inches per minute takes a lot of processing power, but hobby machines would never go that fast anyways so I doubt there will be any problems.

[Mad Welder]

Anyway - this works great on the real VMC's, but what .....does it mean for us garage guys with our Modded RF45's and such. Have any of you guys played around with these types of tool paths.....

While doing my research into CAD/CAM packages last year I downloaded pretty much all the available evaluations and while it’s not HSM I settled for the Rhino 4.0 Rhino 4 New Features and the RhinoCAM2.0 pluginRhinoCAM - Affordable Integrated CAM Software for CNC machining for Rhinoceros CAD Software and MecSoft is fairly close to releasing the new Rhino 5.0 Rhino 5.0 90-Day Evaluation 2012-04-17 Download

There is a small learning curve to exploit RhinoCAM2.0 to its full capability (as opposed to some of the excellent videos of air cutting I seen)…. and with a little tweaking and trials on my own conversion to see what Feeds and Speeds really works I can honestly say it’s as good a CAM package you’ll get for us "Garage Guy's" but it’s not HSM…… however, as I get more familiar with what really works with the machine I have reduced machining time approx 50% since I first started generating toolpaths….you have quite a good array of input parameters which also reduce machining time when applied correctly…..

As I said it's not HSM but it is really worth looking at while you're researching...

Good luck with your research…..

[LAKESNAKE]

I'm using HSMworks on a benchtop machine, and being able to use the full length of the tool to cut saves a lot of time in my limited experience. Here's a video using a cheap end mill (the kind that come in a box set). I was amazed at how deep I could go without breaking a tool.

http://www.youtube.com/watch?v=w0aJn5HHh7M]cnc 2 - YouTube

[RTTIM]

After playing around with parts for work over the last year or two, I have to say that generating stock of the correct size for a given part consumes the vast majority of machining time and causes the greatest wear on tooling. For me, that almost always involves cutting a block first on the band saw, then on the mill to a specific and (usually) rectangular dimension.

I can see where this could be an issue. Won't have my new cnc mill set up until the end of next week, but for my manual projects I've always cut the blanks manually. I have both a metal band saw and 14" cutoff saw, so it hasn't been an issue.

To avoid excessive waste, I try to get the raw material in a size that requires minimal machining. For example, one part I do fairly frequently is roughly 2.75"x4"x1/2" - I buy 3"x1/2" bar stock in 6 ft lengths & chop the blanks to length.

I also frequently shop the "odds & ends" room at our local nonferrous metals warehouse and am often able to find useful lengths of material at the same or sometimes even slightly less cost/lb than if purchased in stock lengths. They will also do custom cutting, and if you keep it simple the cost per cut is reasonable.

Tim

[RTTIM]

I've previously done all my designs in Turbocad, but just purchased BobCad/CAM v.24 and am in the process of converting everything over. It's a really nice user interface - just have to get used to it. The setups seem to be straightforward and I can see where the ability to customize the post-processor could be very useful.

There are a number of toolpath options - will just have to play with them and see which works best.

Tim

[jid2]

Flenser - I have been thinking about this mentally as I'm still not up and running, but I believe you need a totally new process for making parts. What you do on a CNC vs the manual mill are hardly related. I believe that with good CNC workflow you should not be sizing your billets at all, and you actually want the stock to be a fair amount larger than the actual part. This allows for clamping, profiling, flipping, tabs etc. Time is money, and if a slightly larger hunk of stock allows you to eliminate the labor-sink of billet sizing than that's what you do. Perhaps a more experienced CNC wizard can confirm this.

Unless you are making parts that are at the envelope of your working area, or too deep to profile with an extended cutter all that can be done with the toolpaths.

As for me and CAM, I plan on sticking to Gold certified Solidworks integrated packages, and HSMWorks is my favorite so far. I've also tried SolidCam which is 2nd on my list and CamWorks, which I have the install media and due to the fact they had to send it to me via mail I consider them behind the times. I might install it - but probably not. Visual Mill was nice to use but lacked power and integration, BobCAM was hard to use and not well integrated either. The fact that HSMWorks is giving out a very powerful 2D CAM package for free to Solidworks users is pretty awesome and I really like their software.

[TXFred]

Flenser - I have been thinking about this mentally as I'm still not up and running, but I believe you need a totally new process for making parts. What you do on a CNC vs the manual mill are hardly related. I believe that with good CNC workflow you should not be sizing your billets at all, and you actually want the stock to be a fair amount larger than the actual part. This allows for clamping, profiling, flipping, tabs etc. Time is money, and if a slightly larger hunk of stock allows you to eliminate the labor-sink of billet sizing than that's what you do. Perhaps a more experienced CNC wizard can confirm this.

While I am not a wizard by any means, I can confirm that you are correct in your assessment.

I try to design my parts to be smaller than a whole inch dimension. For instance, a piece might be 2.950" x 1.900" x .800". This lets me buy 1" x 2" stock, cut it into 3" pieces, and let the machine shape it. It saves time, and it reduces the possibility of making a parallelogram shaped part.

Conversely, if I designed the same part to be 3.000" x 2.000" x 1.000" then I would be forced to buy 3.5" x 2.5" x 1.5" stock. And that would be extremely wasteful.

For example, here's some sample screenshots of a program to make a soft jaw for a 6" vise.

Image 1 is the stock, mounted in the vise and positioned by visually aligning the left end with the left edge of the vise jaw. Since the stock is oversize, positioning it by eyeball is an acceptable method. The stock is thicker in Z than the final part so that the vise has something to grab onto.



Image 2 is the part after Op 1 is complete. The part has been faced, profiled, drilled, pocketed and chamfered. Only one face, the back side, remains to be machined. All of the other major features were done in a single operation, so they are as good as the machine that they're made on.



Image 3 is the completed part. The part was flipped, and positioned in a second vise with a work stop to locate it in X. A second work offset is used for the second operation. The last side has been faced, and the remaining edges have been chamfered.



So that's a completed part taken straight from a bandsaw cut piece of rough stock. It made a lot of chips, but those can be sold back to the scrapyard. Time is money, and this method saves a lot of time.

Frederic