It could be that the source path got deselected. When you look at the Cut Parameters page, the source path is highlighted in the tree dialog. If you click on the "Properties" branch in that tree dialog, the source path will be deselected and will remain unselected when you green check out. Now regen the path and you'll get that failure message. If you go back into the Cut Parameters page, it will reselect the first operation in the tree so it is a bit hard to deduce what is going wrong. This just got logged as D-29224. Minimally, I need to put better error messaging in. (This is in HST-Project but there may be similar behavior in finish/project or any path with a tree dialog on a parameter page)

Those operations are marked for "batch" processing (at a later time). Go into your parameters and go to the tool page and look in the lower left for the "To batch" checkbox. Uncheck that and save parameters (and regenerate).

Wow, create an offset of that surface. With an offset distance of 0.25 (equal to your tool radius). That offset doesn't look so good (twists in on itself).

I think your figuring is correct - I think a 0 would be the same as "use as computed". Right, with a ball cutter, the stock model option still has an "ignore" limit (the tool radius). I need to dig in, a bit, to better understand what its doing.

D-35179. Here's my sample part to show the issue. Point Optirest to the stock model operation and regen and you get the error message (and no path). Point Optirest to the source path (rough/pocket in this case) and regen and you get a path. optiIgnoreSmallCusps.zip

For optirest, if the stock shape is defined by a stock model operation (the OneOther operation happens to be a stock model operation) OR by a CAD file (STL for example) then the ignore small cusps is limited to the tool's corner radius. So, if you are using a flat end mill (zero corner radius), there is no negative stock adjustment available. I suppose you could try to use a tool with a nonzero corner radius (to allow for some negative stock adjustment). You could try defining the stock shape by all previous operations (all groups, all in machine group or just those in the current toolpath group) or by just OneOther operation (which is not a stock model operation - an Optirough, for example). With that definition, you should be able to use a fairly "large" negative stock adjustment. Effectively, when you ask to ignore small cusps, the stock shape is shrunk inwardly by the ignore distance. When you ask to mill small cusps, the stock shape is expanded outwardly by the mill distance. There are differing methods available to shrink / expand the stock shape - we may choose different ones in different situations. Seems like the one chosen for Optirest has a shrink limit. I don't see this issue logged as something for us to improve. I'll put together a sample part and log it. Thanks for the idea.

Thanks for bringing this issue to our attention. It looks to me like the cutter comp and position code fields, in the binary nci, have uninitialized values in them, in MC2018 (and MC2019) when the Trochoidal Motion/Minimize Burial option is used. I just used 2D HST Area mill and a rectangle with Trochoidal motion to see the issue. I logged this as D-30834. The binary nci records, with Trochoidal motion turned off, look good. I think the problem is limited to 2D HST (the cutter comp and position code fields in 3D HST Area roughing look good).

Yes, there is a switch to reverse the cut order (cut left to right). It appears on the Cut pattern page in our upcoming MC2018 release. Works fine.

In MC2017, I was able to set Rotary 4-axis path to use Left side as the Planes/Working coordinate system (Top for Tool plane and Comp / construction plane) and set the Tool axis control / Rotary axis to "Z axis". And I picked the 4 axis point (on axis of rotation). My path cuts from left to right. But those same settings might encounter a bug in X9. (I'll hunt around in the underlying source code to see if there is a reverse order switch that could be exposed.) I agree, Multi-surface, Cylinder pattern might be your X9 work-around (and offer more control options).

Also, on the third tab page, there is a "Gap settings..." pushbutton. In there, you'll be able to set tangential arc / tangential line.

Thanks for the picture of your part. You are right - no check geometry in rough/pocket. You'll likely need to extend the part along its length (both directions) to keep the tool from rolling around and cutting the sides. You can turn off the roughing passes and turn on finish passes (with multiple finish passes) to rough out the shape but avoid all the air cutting. Finish/contour would work nicely for you (it allows check geometry!) but you only get one finish pass. I suppose you could create several (3, 4?) finish/contour operations each with successively less stock to leave.to rough out the shape. (Surface/rgh/restmill doesn't support undercut cutters.)

You might try the MedialAxis C-Hook. I was able to get it to work on your part. I scaled the geometry up 10x and retrimmed some arc/lines to close gaps in the chain.

Yes, rough/flowline does not support undercutting. It finds the "finish" flow cut and then creates roughing passes from the top down to the "finish" flow cut. This doesn't work when there are undercut areas (you want the "rough" steps to start below and step up). When you enable "check flowline cut for gouge" then the "finish" flow cut has the undercut portions trimmed away. The rough cuts allow you to rough out the top (convex) portion of the part. If you uncheck "check flowline..." then the undercut portions are kept and the resulting rough cuts machine the entire part away. For some time, I've considered adding a warning about undercutting not being supported in rough/flowline. I was going to tie the warning message to the undercut tool (slot, lollipop, dove mill). But, as you point out here, the message should come out even with a convex cutter shape (bull, ball, flat) when "check flowline..." is unchecked. You might get what you are looking for if you use rough/pocket and an undercut tool shape (particularly if you give it an explicit entry point).

Undercutting is not supported in rough/flowline. The roughing passes are always built above the flowline pass. (When you are undercutting, you want the rough passes below [or to the side of] the flowline pass.) There are probably several ways to get what you want - you can make multiple finish/flowline paths, with successively smaller stock to leave. You can create multiple finish/contour operations, with successively smaller stock to leave. You can create a rough/pocket operation (it supports undercuts - the rough passes are offset to the side) but you might have some air cuts.

In Toolpath/Surface/Rough/Restmill, the selection for the CAD file (STLfile) is on the 2nd tab page in the geometry selection pushbutton (or in the geometry selection branch of the Toolpath Manager tree). You can select a CAD file (STL file) and use it as drive geometry or as rest material. I agree with Colin - 3D HST Dynamic Optirough referencing a Stock model operation is a better way to go. I'm glad it worked for you.

Add a check surface to your surface/finish/pencil path and regen. Now the "direction" settings will get applied (and you can set them to begin along your green line.) The check surface can be something far away from your machining area. Why does this work? With no check geometry, surface/finish/pencil uses the same toolpath creation algorithm as 3D HST Pencil - which does not support the "direction" settings. With check geometry present, surface finish pencil uses a different toolpath creation algorithm (one that supports "direction" settings). Minimally, we should put up a warning message that "direction" settings will not be used in a situation like yours. I'll log that as a request.

Something like 2018

Are you using incremental Reference points and do you have the Arc filter (or Smoothing) enabled? I investigated a bug, recently, where that combination led to an extra move.

Try it in MC2017. In X5, we lost profile tolerance and offset tolerance formulas when the controls moved back to the Cut parameters dialog page. In X6, we lost formula files altogether. The formula files are back in MC2017, mostly, but the profile and offset tolerance likely won't be back until the release after MC2017. MC2017 formula files apply to some HST strategies but not all - Area roughing, yes, but not Dynamic OptiRough.

No. I'll guess that the crash corrupted the file's internal time stamp. If the internal time stamp is just an integer then "0" maps to January 1, 1970. +500 maps to some time later that day. +1457028668 maps to a few minutes ago (March 3, 2016). I'll bet that the corrupted file time stamp was some negative number. Then the final calculation (converting Unix time to the Day, Month, Year, Hour : Minute : Second format) came up with that time just before January 1, 1970 (the zero hour). It went back in time!

Time in computers is often measured as the number of seconds from January 1, 1970. Called Unix time.

In surface/rough/plunge, there is also a "Cut depths..." push button. With that, you can set your cutting depths to absolute and set your top depth and bottom depth where you wish. I think the default cut depths might be incremental.

Your containment boundary is a spline. Recreate it as lines and you will get the path you wish. This is a bug - it has been logged as D-09438 "Linearizing containment dropping points causing undesirable toolpath results" I'll add this part to that bug (for testing, once it gets repaired).

You might be able to compress the STL file by doing this - create a stock model operation, set the initial stock shape to the STL file and set the initial stock shape tolerance quite large. The resulting stock model might have fewer triangles. You can then save the stock model out as a new STL file (right mouse menu). (Or consider using the stock model operation in HST-Opti!)

I guessed you were using Classic backplot. Are you using new backplot? When you start backplot, does a separate graphics window appear?