I should have been more precise, sorry, ... yep, the 2nd to last icon at the top of my Mastercam screen is the statistics button (sigma), too. I should have stated 2nd to last on the backplot dialog. It is on the backplot dialog that you can enable/disable quick verify. And then I should have stated the last pushbutton could be used to set the color of the quick verify (in setup). But that would have only helped you set the color in this session of Mastercam. Once you exited, your color choice would be lost (revert back to default). So you are on a better path... in settings/configuration, use the "Backplot" settings rather than the "Color" settings. There you will see "colors" in the middle right and a dropdown list, starting with rapid color. Change the drop down to "verify color".

You might be looking for classic backplot's quick verify. There is a push button to toggle this feature on/off (2nd to last, in the top row). The default color is probably gray. You can use the options push button (last, in the top row) to set the color - use verify color.

Select an existing operation that shows the animation... use the right mouse menu in the Toolpaths manager and select "edit selected operations" and "edit common parameters". Tick the checkbox next to "tool display". A dialog pops up. Close that dialog. Then use the dropdown list to the right and select "Disable". Green check out. Regenerate operation. Does the animation go away?

Ben K is correct - if you select a solid face with two holes (like this one) for your machining region, the path will extract three loops and machine all three independently. In this case, unfortunately, the ordering is such that the two holes are machined first then the outer loop. Ben's suggestion is on target- just select the outer loop as your machining region. It works this way for solid faces and for wireframe area selection. And it works this way, too, in X6 and X7 multiple region (not single region). This is a good part to show the issue; I'll share it with my team to see if we can provide better assistance (a warning message or better machining order). Thanks, Bill B

I got 5 minutes with 0.0001 scallop height and 0.0010 tolerance.

3 minutes 41 seconds on my machine to regen this HST-Scallop as filed. That is using cut tolerance 4.8%, line/arc filter tolerance 90.2% and smoothing 5%. If I slide to cut tolerance 25%, line/arc filter tolerance 71.25% and smoothing 3.75% then it only takes 16 seconds to regenerate. With the looser cut tolerance (same total tolerance), the path size grows from 574K to 856K.

...or, better, see Aaron's answer to the same question over on forum.mastercam.com.

You've generated a tp/srf/rgh/restmill operation and it computed a stock model and it created a path to cut that stock, yes, and now you wish to see the stock that it created? If you navigate to your Mastercam "temp" directory, you will see this stock saved off as an STL file (tmpzrest.stl). It just saves off the stock for the last restmill regenerated. My "temp" directory is c:\users\web\AppData\Local\Temp\Mastercam X8\T0UM0F7EWF - you get an automatically named temporary subdirectory for each Mastercam session - just sort by data modified. I merged this STL into my part file.

Hi, The message is still in X8. But you seemed to have uncovered an issue. I have an X6 part with an HST operation with no holder checking, no holder. I open the part in X8 and turn on holder checking (default holder) and clearance on bottom and regen and I do not get the warning. More troubling - it seems to have not checked the holder. As a work-around, I selected a different holder, saved the parameters, then went back and reselected the original (default) holder. Now when I regen, I get the message and the motion is clipped to avoid holder collision. I will submit this as a defect. If you wish, post your part or email to me (or QC Inbox). Thanks, Bill B

Hi, Operation #1 in your part has arc filter turned off and it regens on my computer quite quickly. Operation #2 has arc filter turned on, at 5% for cut tolerance and 95% for arc fitting and it takes a long time to process. I moved the slider to a 30% - 70% position and regenerated and it regenerated relatively briskly and output arcs for the motion. To get the fullest arc fitting, you'll need a filter tolerance slightly larger than the cut tolerance but they can be pretty close. 45% / 55% or 49% / 51% might do the trick. Oh, and, yes, classic surface toolpaths are not multithreaded and still process in the main thread, so, patience might be required. If things are just taking time, you can press ESC to terminate processing. Bill

Hi, I was able to download this part. It does sort of look like the optimize checkbox is stuck in the "on" position in this path. I'll take a closer look (and forward to QC, if necessary). Bill

Hi, The "smoother" rapid gouge? Perhaps this operation was created in X7MU1 without the smoothing hotfix. That would put rapid gouge in. When you regenerate this operation in X7MU2 (or X7MU1 with the smoothing hotfix) the rapid gouge is not there. Regards, Bill

For the previous issue, remodeling the surface allowed the dogleg rapid issue to go away because the original surface had a little bump/dip/cusp (something) in it that led to a little gap in the raw flowline pass along it. The gap led to a retract/plunge move which led to the smoothing spurious rapid bug (which led to the dogleg rapid gouge). Phew! The advice you got to change your gap size to keep the tool down in the gap was good advice. It avoids the smoothing bug on this part. But I'm worried the smoothing bug is still there lurking. Installing the hotfix (or reinstalling X7MU1) or keeping smoothing disabled will help (until X7MU2 or X8 is released and installed). For this rough/flowline issue, you wish to (rough) machine between -0.30904 and -1.0 but you are getting cuts above -0.30904. If you uncheck the "allow positive..." and "allow negative..." Z motion along surface checkboxes and regen then the rough cuts are contained to your depth limits. It looks like the "positive" or "negative" Z motion along surface is not trimmed to the cut depth limits. Should it be? Well, that might be a good question. In this case, the Z motion along the surface happens to be "flat" (i.e. both positive and negative). Another work-around might be to add a check surface over the area you don't wish to cut.

Hi, I'll take a look. By the way, did you resolve that dogleg gouge issue in op#3 flowline? Did you disable smoothing or install the smoothing hotfix? Bill

Hi, I notice that op #3 has smoothing enabled. You might have X7MU1 installed without the smoothing hotfix. If you disable smoothing in op #3 and regen, does the dogleg rapid gouge in verify go away? If so, consider reinstalling X7MU1 (with the hotfix) or keep disabling smoothing until X7MU2 or X8 is released. Classic backplot doesn't show the dogleg rapids; you can configure X7MU1 to use the new backplot. New backplot shows the dogleg rapid motion (it matches verify). Regards, Bill

Hi, I can explain this one. You have the Tool containment "Total offset" check box checked. This excludes the tool shape from the inward offset of the containment boundary. If you uncheck this check box and regenerate the rough/pocket operation then the tool stays inside the tool containment boundary (and inside by your additional 0.01 offset). When you uncheck the check box, you might notice the dialog control changes to "Additional offset". This adds half the tool diameter to the offset which keeps the tool inside. I'll see if we can add more information about this check box to the Help / Field definitions. -Bill

The check and drive status of surfaces is different in version 8 than in version 9. In version 8, you need to do 3 things, mark 'em, pick 'em, and use 'em. You need to mark the surface as drive or check, you need to select all drive or check surfaces you want to be processed in a given operation, and you need to check the "use check surfaces" checkbox to actually distinguish check surfaces from drive surfaces. Whew. In version 9, you no longer need to mark the surface as check or drive and the "use check surfaces" checkbox is gone. You only need to select it as either a drive or a check. Much easier. Rough/pocket does not (and has never) used check surfaces in its processing. In version 8, you can mark a surface as check and add it to the operation but you cannot enable the "use check surface" checkbox, so the check surface will be treated as a drive surface. (In the geometry menu, the number of drive and check surfaces are listed but you have to look at the "ON" or "OFF" keyword after the check surface count to see if the check surfaces will be treated as "check" or "drive", respectively.) If you save, from v8, the .mc8 file with a rough/pocket operation which has check surfaces (but doesn't use them) and bring the .mc8 file up into v9, you will see that the operation will now have only drive surfaces listed in the geometry menu. Why does rough/pocket not allow check surfaces? A check surface is one that you do not want to machine. But rough/pocket machines all surfaces forming a pocket. So there is no difference between it and a drive surface. You might argue that rough pocket should allow check surfaces so that you can specify zero offset on flat floors and positive offset on walls (or vice versa). This is a valid request but the drive and check stock are 3d values (applied in all directions about a surface). So you won't quite get what you want. What you need is a flat surface machining function (look for a chook to be released shortly after version 9.1!)