That is mostly for simultanious 5 axis work. Since you have the Variaxis J series, which is not capable of full 5 it shouldn't be to big of a deal. You may find that certain paths won't work that need to be driven from the tip of the tool. Best bet on this is to talk to Mazak/Mastercam and have them let you know what is driven from TCPC. If you are only doing positional work don't even worry about it, you don't need it.

G68.2 is Tilted Working Plane. G54.2 is dynamic work offset, and G54.4 is Work position error.

You can still set min/max, although I haven't used the older Mcam. I believe what you're looking for is under steep/shallow. Check "Use Z depths" then the options become available. Rereading your post. You don't actually have to draw additional geo with this setting. You just set the height you want in the steep/shallow

There are 2 different ways to accomplish this with the machine. The older way which is to program from the center line of rotation on the machine. Both Mastercam and the Variaxis would have G54 set to centerline. Then there is G68.2 (Tilted Working Plane) and TCPC (Tool Center Point Control) which automatically handles the WCS as the rotaries move. The second way is definitely easier and creates better work flow both in the machine and on MC. However, rotational issues are slightly harder to diagnose. It's not always as simple as adding another WCS. If you have a strong understanding of the kinematics it won't be to bad, or if your parts are generally wide open. Both of the above solutions are handled by the machine. There isn't really a way of getting Mastercam to handle this. As machines change slightly from day to day it's not really a good idea. If you do go the G68.2 route make sure your machine came with the option before pushing for it in the Post. Here is a video of how it works on Haas machines. Note the codes are slightly different, but do the same thing.

Motor-Vater. The easiest way to use a very specific plane that I have found in the multi-axis paths is to use conical limits. Draw a line of the z axis direction of the plane you want. Turn on limits under tool axis control. In the dialog for limits turn on conical and limit the angle to the defined line. Then if you want 3 axis, type in 0 in both fields. If you want movement give it the limits you want to use.

There is indeed. Here is a link to the section http://forum.mastercam.com/Topic24914.aspx

1. Can be done. I have my computer setup this way Open, File/Configuration/Toolpaths/ Check box for Lock Feedrates unchecked. It should now update everytime you select a different tool. It's a huge pain on lathe tools, but a must have on mill tools. 2. I believe what you're looking for is also possible. Open, File/Configuration/ Toolpaths Manager/ NC File hit the Last Operation's NC File button. I don't use this setting, so I'm not sure if this is what you're looking for. If it does work let me know, I might change to using that instead. Hope this helps you both. Caleb

Draw a circle the size of your drill and where it starts. Then define that chain as an air region. It should pick this point automatically as long as the hole is large enough, and the entry page info is set correctly.

I would highly recommend updating to 2019 if you can. The 3D lathe tooling is way better. Describing the tools can be cumbersome. But not having to draw tools is amazing! I also run an Integrex, sweet machines!

In tool designer, compensation, what method are you using? Corner,Center,Tip,Edge are the options.

What toolpath are you using. Some are not compatible with tilt to avoid.

I face the same problem at the shop I work at. One of the guys flat out refuses to use the probe at all. I've questioned him on it a couple of times and it sounds like a trust/training issue. He's been provided the the means to use it, he just won't. Has a edge finder and a indicol setup all the time. It's absolute insanity considering all the benefits to using the probe. But, what are we gonna do, they're machinist...

Two other things I can think of. In the tool page, on the probe, it could have a model of the probe drawn up for it to use for collision detection. You can either delete or modify it to work, although I've never modified one before. It would say something in the bottom left corner. The only reason I could think of for this to change is a different probe length. If you changed the probe recently this might be the problem. The other thing I can think of is if the machine was setup with a 4th axis. They would have drawn and defined its position in the parameters. If you've taken out or moved the 4th recently this could also be a problem. I'm not exactly sure how to change those settings, but it should be easy enough to look up in the book. There is a way to bypass the problem if you can't find a fix and need to do something now. It will most likely be on the main page or tabbing right. The button is called "Safety Shield" you can turn these off and it won't check for collisions. (Upon looking at these you can actually turn collision checking settings off individually. You can narrow down what is causing you problems by shutting one off at a time and seeing where it's getting hung up.)

It should be 1 or 2 tabs to the left. It will say "set up info." Open this tab and make sure everything is cleared out. It holds onto this info and can use it during both EIA and Mazatrol. The purpose is to draw exactly what you're working with so the tools don't collide with stock.

I run a Integrex with the new Smoothx control, but I've got a similar alarm before. It had to do with the set up info. page. I had material designed in this and a mazatrol program in the main memory and was trying to run tape. It kept "running into stock" I had to blank out the set up info. fields and change the main memory program to an eia program. I'm not sure which one actually fixed the problem as I changed both at the same time.

Here is a picture (Pencil Stutter) of the sharp edges I spoke of, I took a screen shot and outlined what I was talking about in red. If you zoom in on these sections in MC you can see the sudden direction changes. This is a result of the way Pencil is processed. It is offsetting internal corner radii. I have attached a pdf of the offsetting I'm talking about. When you look at it, the left side is the original line that I drew and as the lines are offset in eventually a radii becomes a sharp corner. This is why pencil isn't really the best at surfacing a whole part. It's more designed to pick out corners left behind by other paths. Hope this helps. Caleb PENCIL STUTTER.BMP Sample Offset.pdf

Lucas, I took a look at the file. I can see that in some parts of the path it has extremely jagged edges, this is a result of the pencil toolpath which really isn't designed to be surfacing a surface like this. You mentioned in your post something about scallop so I'm guessing this might not be the path you're using. Even the bigger and better machines out there can't handle the sudden change in direction that the toolpath you had is showing. Most machines only slow down when they see arcs and try to maintain feed on line segments. Your machine may be doing the same thing. I did try a couple of different paths against the part that I was confidant would do a bit cleaner job. First off is Equal Scallop which is a new toolpath in 2019. I saw that the file you posted was in 2018 so I'm not sure if you have that yet. If you don't you could try the Raster path, this is slightly less efficient then the scallop and takes some kindy funky parameters to make sure it doesn't skip over large portions of near vertical walls, but it provides you with basically straight lines instead of arcs all the way across the path, only changing direction when it loops off of the part. Hopefully keeping the tool from stuttering while in contact with it.

There should be a much simpler way of handling breaking up the segments into the length you want. You can just draw a normal circle and do a contour path (or really any path.) Open up the Parameters: Arc Filter/Tolerance: Check smoothing settings: Check Use Fixed Segment Length: Then type the length you want in the box. Looking through this page there may be some settings that will help you that I have never had to use before. What jumps out to me is the Override Arc Feed Rate. You could try decreasing the Max ID Decrease to something like 20 IPM so that instead of relying on the machine to take care of Acc./Dcc. your overriding the feedrate to something the machine can handle.

I do the same thing, no reason to have wireframe cluttering up the screen and directly linked to the paths. The use of push/pull accomplishes the same thing much faster, without the need for wireframe.

Sorry about the response time, I had to leave work early on Friday and wasn't done thinking about the problem yet. After rereading your original post I figured there might be one other factor. Starvation. There is a machine limitation to how fast it can read code. This problem becomes worse when you have to drip feed. In the shop I work at we have some older Mori Sekis which can't run any of the HSM toolpaths faster then around 40 ipm because it will start to starve the machine and jerk around. This could be an issue if your machine can't read code fast enough. A complicated question. The definition of high speed toolpaths differ depending on what person/company you talk to. I personally think of High Speed toolpaths as anything that is taking full advantage of the machine/tool you're using I.e. D.O.C., SFM, Axial/Radial load, chip thinning, etc. However, the definition is a bit convoluted. A lot of the 3D toolpaths are high speed paths (except pocket), at least by Mastercams definition. Most of the 2d paths are not (except the toolpaths with a red and white arrow.) It sounds like your problem is narrowed down to one of two things. Either your machine is starving, or your post is not posting out the high speed options (if your machine is capable of them.) Fixes: Starvation: If your machine truly can't keep up with the code thrown at it there are a couple of options to help it out. Better settings optimized for longer code segments on your Arc Filter/ Tolerance page. You can slow down the feed rate to the point where the machine can actually keep ahead of the smaller segments of code. If you're running drip feed you could try to find a way to get the program loaded onto the machine. such as breaking the file into several programs. High Accuracy: You can call the manufacturer of the machine and ask them if there is a better setting to control Acc./Dcc. Another bit of code I though of is G5 P2 which enables further look ahead then G61.1. You could also look through the manual to see if you can find any of these settings or maybe settings specifically for your machine. Sorry if this isn't much help as I've never heard of the brand of machine you're working with.

Not sure what brand of machine you're running, but most machines need a "high accuracy" mode to control acc./dcc. I run Mazaks at the shop I work at and this is controlled with a G61.1, KX. You should have a similar setting on your machine, code just depends on the brand. This will control the look ahead of the machine and how it handles speeding up and slowing down when the machine sees an arc. If you can name the brand of machine you're working with someone might be able to provide the info you're looking for.

Open up the tool manager and right click on the 1/4-28, edit tool, avoid setting a standard size and instead type in .125 in the Nominal diameter field and 27 in the threads per inch field. Adjust the rest of the tool if you want, but these two edits should make the tool work as you need.

I've been using it quite a bit, but only on AL. Impact on turning times is not huge, but does exist. I'm seeing much better times, mostly due to switching to round inserts that are capable of turning on both sides large flanges. Just as a warning, there are some pretty serious issues with it currently depending on what you're doing. Because it's based off of peel mill it likes to wrap around the ends of your parts, it does not respect clearance angles, does not like rest machining very much at all and, due to it always looking at stock that path will sometimes generate paths far away from the geometry you actually selected. All of these things require quite a bit of extra wireframe to be drawn. There are also a couple of other things I've had to consider since starting to use it, such as switching to constant rpm instead of CSS in certain situations due to using round inserts your feed will typically be extremely high. This means that in certain areas of my part where the tool dives nearly straight up and down in X that the spindle load stays around %150-%200 with CSS. If you need some help with any of these problems I have found work around for nearly everything mentioned above, just let me know Caleb

Hi all, At the shop I work at we use warm up programs every day. I've been slowly rewriting them across the shop as the original programs were dumped long ago. In order to simplify the programs I've been using variables to write them. Seeing if I could not only make the programs smaller, but also make them a little bit safer to run when a large piece of material is loaded in the machine. I recently added something in to the program that tellls the machine the max tool length that can be used to run the program and figured I would post the whole thing on here in case that someone has lost the original program or needs something different to modify. O9999(WARM UP MAIN) (WARM UP) IF [#[60000+#51999]]GE[7.0]GOTO9000 (This line checks the tool length before running the program, modify the ([7.0]) line to the length desired before running. #650=1000 (This line defines the starting spindle speed.) #660=8000 (This line defines the max spindle speed for the machine, when it hits this number it will start over.) G00 G28 G91 Z0. G28 X0. Y0. WHILE [#650LE#660] DO1 S#650 M03 G01 X-19.69 Y-16.93 Z-5. F150. Y16.93 Z5. X19.69 Y-16.93 Z-5. Y16.93 Z5. #650=#650+500 (This line defines the increments for which the spindle speed moves up in, until reaching the max and starting over.) END1 M99 N9000 #3000=21 (TOOL_LENGTH_CAUTION) (Custom alarm status, Write into the parenthesis desired alarm.) Note that the machine this was wrote for could move down 13" before hitting anything, so I wrote in 7" as the max length to minus the 5" it moves down in Z plus 1" of clearance. Also note that this program was wrote for Mazaks only, please do not attempt to run on a different brand of machine as the variable numbers will vary.

Use Steep/Shallow: Use Z depths checked, and set the maximum material below the part what ever you want it to come down.