toolpath transform mirror should force you to set the "source" to "geometry", but there is an issue and it allows you leave the "source" set to "NCI" which will not give you what your looking for. So set the "source" to geometry and you also have some settings on mirror page for "cutting direction" which should allow you to get the results your looking for, usually have this set to maintain start entity. If you are doing a lot of deburring of edges with a ball endmill use the "curve 5 axis" toolpath. This works very well and is easy to program, basically it's a contour toolpath that can compensate to surfaces. If you don't have access to it have your dealer show it to you.

I believe the default active reports setup sheet will list out all the operations that a tool is used in.

any of the methods other than using a tool will look for cusps or steps left in the material. Using tool will basically only look at internal corners. The ignore small cusps is what you need to use. it doesn't take much of a cusp to be .020" thick. I usually set my ignore value to slightly less than programmed stepover and get reasonably good results. But again it's supposed to be looking at where material is left behind based on where the previous tool cut or a stock model so you will get cuts in those areas. HTH

curve 5 axis toolpath can lead in left or right relative to cut direction. So if you have the multiaxis or curve/drill 5 axis functionality you can do this. Does Dynamic Contour not give the lead in motion you want? I can see for a basic zig zag facing operatioin this would be a good enhancement. - But facing does have dynamic motion as an option.

Have you tried using dynamic contour to get the lead in you are looking for? If I understand what you want it's to keep the chip thin when the cutting edge is leaving the stock and dynamic contour will maintain your chip load.

max radius and profile tolerance only apply to the pass closest to the geometry. they also only apply to internal corners (you won't gouge your part on an external sharp corner) offset tolerance applies to all other passes. as stated how you use them depends on the machine and what your goals are for the toolpath, do you want it to remove all the material it can, or do you want it to run smooth and remove "most" of the material it can. some generic values that I used as starting points before opti-rest max radius = 10% of cutter dia profile tol = 5% offset tol = 10% . . . but really just use opti-rest you will be much happier with the results.

use fbm drill to create tool engagement vectors and points. Then create a 5 axis drill toolpath to all the holes.

It's easy to throw the end user under the bus, as the problem is not mastercam. but it also may not be his/her fault, doing the best they know how and not getting good results does not mean software or the end user is bad. Just some training is in order. And if the trainer isn't real familiar with the type of work you are doing maybe some consulting from someone who is. A .2mm endmill is delicate, so should be the approach to material removal.

I wiish I had all the time back I went through prints with different color highlighters so you could easily identify different types of dimensions at a glance (Significant/critical, positive stock/negative stock, etc...). Digging through hundreds of dimensions to identify 5 "significant" and "critical" dimensions is painful. Critical dimension prints have been a useful intermediate step on our way to full MBD.

The Roeders does not like arcs, in fact the more consistantly spaced code the better for finishing toolpaths. Try a .0002" total tolerance set to 50/50 utilizing the fixed segment length (which is actually a max distance length). Then you have RMAX, RADMAX, etc... to smooth out the program at the machine.

a simple 2d pocket with roughing disabled will ensure no chain is violated.

For those that need to do this type of work on a regular basis I have recommended people purchase the curve and drill 5 axis toolpaths just as "Teh Bear" mentioned. It's incredibly simple to do with the curve 5 axis toolpath. Basically a contour toolpath with surface compensation.

Thank you Greyman, this isn't for me but one of our customers. I'll send this thread to him as I haven't been in front of an EZ TRAK for well over a decade. Thanks again,

Can someone enlighten me on how to use cutter comp at the control on a Bridgeport EZ TRAK? Anything special to do in Mastercam for lead in lead out, or do I not program the lead in/lead out in mastercam at all? Can I use cutter comp when posting out gcode or just conversational code? Thank you,

To be honest your never going to get it perfect. Via setup sheets you can scale the cycle time to reflect an average deviation percentage to get you fairly close. I shoot for being within 3% on average. There are just too many variables that affect the run time. For example, a program ran on a haas had a backplot time of ~5:00, run time of ~7:30. Add a G187 for "roughing" and the run time drops to ~6:00. So even the same code, on the same machine can be drastically different. come up with as consistent a process as possible, track setup sheet run time compared to actual and then edit the setup sheet to reflect the average deviation. hope this helps,

nobody's pretending anything. I send things in all the time, and I try to lay out exactly what I'm looking for and why. Many things get fixed, enhanced, improved, or whatever else you want to call it every version. I do know what you are talking about when it comes to solid chaining a chamfer, it's simply not possible based on the edge you select. it usually requires picking a different edge and using stock to leave or simply using wireframe geometry. But just because I know what you are talking about doesn't mean the developers do, we need to get examples to mastercam for anything to change, period.

Scott, I'll check into the file merge error "no matching opfile" if I remember right, that error is usually tied to using an an updated config file in X5. Have you tried a default config file? As for any other issue, all we can do is show them what and why it needs changing, regardless how many times it has or hasn't been sent in. regards,

Scott, the best thing we can do is send files in to Mastercam than lay out exactly why improvements are needed. Send me a file and we can get lay out exactly why and what needs changing and get it logged as an enhancement request. The more clearly laid out examples of why improvements are needed the better. Regards,

without seeing exactly how your cutting it, it seems really odd that you are breaking tools. Especially at unpredictable intervals. The only place you could be breaking the tool is going into one of the corners. Dynamic contour is a great place to start and let it peel the corner out of there. There are a lot of really good endmills for this from a lot of different companies, polished and coated, like Harvey, ISCAR, Benchmark, etc... Don't be afraid to have a tooling vendor or two come in and try some of their tools. While a speeder would certainly speed things up, you aren't running a sub 1mm cutter. You have 10K for a .125" endmill which should be plenty to eliminate the breakage and speed things up by switching to the dynamic contour. Get a balanced holder, it can be a collet holder, they help a lot with small and smallish cutters.

That was actually very nice functionality back in V9 and earlier, I was disappointed when it was gone in Mastercam X. But, I wouldn't trade the old backplot for the new one in a million years. the ability to rewind and change the speed on the fly is invaluable. But I personally think it's time that backplot received some "love" as it's been relatively unchanged since X came out.

Unfortunately this was functionality we lost with Mastercam X. I do not know of a way to make it do as you would like.

Yes, sort of... nothing makes life easier than having a standard levels list. I actually merge my geometry into a template file that has been setup for a specific type of part, mold base, mold core, electrode, horizontal tombstone, etc... A template file consists of my standard levels, my standard toolpath groups (and sub groups), some standard toolpaths for certain types of parts, standard views (custom views tied to geometry on named levels so than can be easily edited), standard tools pre-loaded into the file, etc...

MN cut stone, you can always contact us directly. I have quite a bit of experience doing these types of cuts. I'm sure you are familiar with Park Industries and their infinity machine with the 48" and larger saw blades. For some general info this is usually done with a swept 2d toolpath. you will need to make some minor modifications to the geometry as the swept 2d will only compensate to the tip or center of your blade and will not account for the blade thickness and the "upper" corner radius. It will compensate for the bottom corner radius correctly, or a full radius. I downloaded your file and put a toolpath on it, contact me if you want me to send to you. Regards,

If your 2d dynamic toolpath is taking a while to crunch, simplify the geometry. A spline with many control points adds a lot of complexity. 1. use the CAD tools mastercam has to simplify a spline or break it into many arcs. 2. the best way is to create a 2d contour with no cutter comp or lead in/lead out. turn on the arc filter at a 2:1 or 3:1 ratio so the toolpath contains mostly arcs. Then backplot the toolpath - save as geometry. Now you have some really nice simply geometry to create your 2d dynamic toolpath with and the calculation time will be significantly less. I've had a 2d dynamic core mill go from 15 minutes down to about 90 seconds by doing this. when you have multiple chains and all of them contain very dense splines the calculation time suffers. HTH

i'm not saying that eliminating the arc's are the solution, not using HPCC is the sollution, or not using cutter comp is the solution. Mostly just trying to find the root cause of the issue so it can be addressed properly.