Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Aaron Eberhard

Verified Members
  • Posts

  • Joined

  • Last visited

  • Days Won


Everything posted by Aaron Eberhard

  1. In general practice, only if I'm doing a clearance pocket (i.e., I actually want circles in the corner so you can remove a plug), and it's <= the endmill diameter. I did have a small aluminum aerospace bracket with pockets I helped with a few years ago that had really thin walls (think RF components, each in their own little "pocket" to keep them isolated). I ended up drilling out the corners before any roughing was done because you could see a bit of distortion bowing out the corners of whatever pocket was done second. Switching to a smaller endmill would have taken care of it, but I ran the numbers on their machine and it was faster to drill out the corners to reduce that load than it was to switch to the smaller mill. There were a lot of pockets I believe it was really an issue of the thru coolant and/or chips pushing on the walls a bit during evac?
  2. Glad to hear you liked it. I really enjoyed it too, it was like sitting with an old friend discussing and learning Absolutely, let's figure out a time in the next few weeks!
  3. You probably have "only display selected toolpaths" turned on:
  4. One thing to be careful of with the Opti/Dynamic toolpaths is to make sure your microlift distance and speed is more reasonable for a linear way modern machine. There's no reason to back off .01" unless you've got a ton of Z axis backlash, .002-.003 should be fine. Max out your back feed rate to whatever the machine can theoretically traverse at. It defaults to 100IPM, which is way too slow, especially since you'll be aiming for >2000 IPM range most likely...
  5. The other reason to default to Dynamic/Opti is that they generally put less stress into the part, if flatness or tolerances are tight on the finish product you'll get a lot less distortion when you unclamp than with traditional methods. You can dial in the amount of load you're putting into the material, and often trade a bit of roughing time to not have to do a second "finishing" op after releasing/skimming/reclamping the part. Sometimes it's not raw toolpath time that's the big win.
  6. Someone responded and it reminded me I never added my other tip to this.. You can drag and drop a Mastercam .mcam (.mcam-operations) file directly onto the Toolpaths Manager and it'll open the import dialog, so you don't even have to go through right-click > import > browse if that's faster for you.
  7. I understand that JB asked this last year, but to answer the question: Pretend you have a part that's floating out in space somewhere (aircraft coordinate system), so you make a new "top" plane called G54. Now, you have to make a Front plane that you call G54 A+90. If you make a toolpath or just have your selection set to G54 / G54 A+90 / G54 A+90, that option would just show it as "Front," which can be less confusing for people. The problem is that a lot of times your planes won't match an existing idea, so then you get Undefined. I prefer properly labeling my planes, so there's no ambiguity, but a lot of people are lazy/sloppy, and this helps them.
  8. Yeah, this is the proper way to do it... You'll potentially lose/break functionality that's been changed/added/removed if you manually copy over the workspace file and it contains references that don't exist anymore.
  9. What size do you need? I recently used an Ingersoll S062T10CA-80 (https://www.ingersoll-imc.com/product/4542998) That's 8" long @ .625 with an indexible end (I used a 3/4" head 12J1D-07008TRR01 (https://ingersoll-imc.com/product?ecatProductId=4461233) for my application. Works great, but I needed it to be smaller. Also, if you do long reach tools, one thing to keep in mind is that you need to have a decent chip load or they'll vibrate. In my example, I figured out to feeds & speeds for a .005" DOC finish pass in 420 Stainless. One of the parts only had .002 or so left, and the surface finish was crap. When it had .005" left, I got a 20RA and .008µ (.0003") flatness. One thing I recently learned is that Haimer (I thought of them primarily as a holder company) is the ones who developed the Duo-Lock interface, now commonly used by Kennametal. Kennametal only offers the duo-lock extensions in "heavy metal," which gives good damping characteristics, but if you really need carbide, you can get it from Haimer.
  10. Correct. It's statistical analysis across the entire population. Glad to hear that you're still getting proportional raises, though, not just cost of living increases!
  11. Yeah, Zaffin_D beat me to it, but all of those options are available if you right click in the random grey area next to the tool list: For anyone on the milling side, they're there in all the old style mill toolpaths, too:
  12. That's not just the CNC programmer market. The other corollary is that statistically, your earning potential is set in your 20s. Thanks to the modern era (1990s onward), it appears you can adjust that into your 30s, but by the time you reach your 40s, your "working for someone else" earning potential is most likely set for the rest of your career. That's also most likely the reason why most (again, statistically) startups are founded by people in their 40s.
  13. If your sides are straight (i.e., not influencing the shape), for something like this, I'd use a Lofted surface. You don't need the straight lines: Note that it will still be two surfaces, as mathematically surfaces can't a sharp intersection and maintain it like in the left little surface. Now, if you want it to be all one surface, your best bet is to put a little fillet between the corner, it doesn't have to be big, .001" will be fine:
  14. Yep. I made a little video to show how to do it:
  15. Axis sub will always give you the cleanest code, but without a toolpath, we'd just be guessing on this one..
  16. Agreed, this is great advice. The other part of this is to really leverage import/export, and set up material specific operation libraries. If you import an operation, you get the correct tool with the feed & speed already loaded, all stepovers/etc. set up, and all you have to do is select geometry. For example, every time you run across a 1/4-20 or M8x1.25, you should be importing all N operations and have your geometry selected so you can choose the first operation, then drag and drop the geometry to the other ops. It should take you less than 30 seconds to get that programmed in any material you've done before. I completely agree with Matthew above. Learn to use wear comp for any finishing passes, and learn how to jump into a program on your control and resume. Make anything critical (especially round bores & bosses) have a separate toolpath for a finish pass with wear comp on, so you can immediately probe your critical feature on the machine, adjust wear comp if necessary and re-run the finish passes. I know a lot of people who re-ran an entire 20 minute program because they never figured out how to jump directly to Op#18. I was just onsite with a customer doing some training and showed them these two things above (toolpath library creation and figuring out how to jump directly to an op on their control) and we estimated that they're going to save at minimum 6 hours of programming and 2-3 hours of machine time per week! Every time they were encountering a 1/4-20, they were defining the tool, setting the speed for the materials, defining the drill toolpath params, etc..
  17. Also, don't forget that you can create a viewsheet with your your levels open, WCS set up, etc. etc., then right click on the view sheet and choose "Save viewsheet bookmark."
  18. In 2023, there's an option that's perfect for this called "tilt relative to reference surface." See the attached picture. For this part in 2022, I'd set it to rotate around axis, with an angular limit around z of +5 to 185 so it doesn't go vertical and cause your C-Axis run away (called Singularity) as DBronson points out.
  19. Looking at the points your spline was made from (create Points > Node Points), then creating lines between them reveals that there's an inconsistent angle between the points, which means you're not going to have a "smooth" spline, as it has to conform to each points different. If this isn't a high tolerance part (and I'm sure it's not as you're only making 9 points across 53"), so I'd recommend just not using the odd points. In this image, I made the orange spline by only using the points from the points indicated by arrows. Much smoother as it doesn't "tuck in" to hit the points not on the "arc" that I want to hit.
  20. A handy way to check whether it's possible to do things is to look at it from the front, switch to 2d mode, create curves on edges (your straight walls) and modify length to see if they intersect the origin. Obviously, on this part it's easy to visually see that it's not gonna happen, but I've seen parts where the wall was only off .5° or so, so it looked like it was possible until you really analyzed it: What Ron's saying, in this example, you have to treat anything between the orange and blue as an undercut feature, as if you were doing an undercut wall on a 3 axis machine.
  21. Glad to hear you got it sorted out :) Yes, they can work with encrypted posts, but you won't be able to see the math behind what it's doing :) That's where you'd need your post writer to include the options that you want. To understand the misc values, think about the machine-specific situations you could be in. For example, you have a trunnion 5 axis table sitting on your vertical mill. The tilt . You need to machine something on the front of the part, so the trunnion needs to rotate the cradle (A axis) either +90 or -90. If it tilts +90, the bottom of the cradle will be facing you. If it tilts -90, the trunnion will be facing the back of the machine, and you can see the part. Either solution is technically correct, and will machine fine, but you'd obviously prefer to see the part being cut @ A+90, right? That's where the Misc Integer "Initial Primary Angle" comes in. If you type in 90 into there, when the post starts to figure out how to move the machine to get to the front face, it will start with the assumption that the A axis should be at +90. Another example would be if your machine has a smoothing setting, say it needs to output M250-M255. You can have a misc integer that lets you control which smoothing setting by typing in 0-5 into that field. Hope this helps!
  22. I would start by reloading the post with Machine Group > files > Replace. Then, I would set your toolpaths to "Automatically set to Post defaults when posting" on the Misc Values page. Finally, I would follow JP's instructions, and have a session with your reseller. Your buddy is wrong, there's many many many times where those values will do anything from improve your surface finish to prevent a crash by orienting your machine the correct way when posting. Learn how to use them.
  23. Yes, there are computer science, math majors, and guys who just started on machines and understood what needed to be done and figured it out behind all of this stuff. All of the CAM software has their wonks behind the scenes doing that. If you want to meet the people behind the curtain you need to be pretty specific about which toolpath you want to know about. For example, there's a different guy behind Mastercam's Dynamic than, say, Equal Scallop. And each toolpath is really a team effort anyway. ModuleWorks in particular was started by Yavuz Murtezaoglu, and he's the guy who wrote the original 5 axis engine for it which does all the surface-based stuff (morph between 2 curves/surfaces, parallel to curves/surfaces, etc.). He's not the guy who actually coded the newer geodesic engine stuff (in Mastercam's Unified toolpath as guides, automatic mode, or Morph/Parallel set to "exact" mode). He's also not the lady behind the Swarf Milling. They now have a lot of programmers! Depending on how far down you want to go, the guys who apply this stuff to make toolpaths are often standing on the shoulders of giants in the fields of Mathmatics. Many toolpath ideas are taken from mathmatics and physics white papers. For example, Yavuz cites Dr. Bronshtein's Handbook of Mathmatics as a fundamental basis for his original toolpaths.
  24. The only thing you can really do is increase your quality (the slider on the lower left), but because verification in simulator is making a triangular mesh model (like an STL, but a bit different), there's not too much you can do. At some point, it will be making lines, not arcs.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

  • Create New...