x9 Dynamic OptiRest cutting from the outside thinks it's pocketing

[dvandewalle]

I apologize if the has already been beat to death elsewhere, but I've dug through the archives and I can't find any data that actually can make this work.  I've used other CAM packages for years, but am fairly new to MCx9 (SP3) and I'm hoping I'm just missing something stupid here.

 

I'm not able to get x9 to generate an opti-rest tool path that doesn't treat the outside roughing of the part like cleaning out a pocket all the way to the containment boundary.

 

I've defined a stock model (and tried a couple different ways to do it), I've set tool containment with large offsets, and tried all sorts of options.  I can't seem to get mastercam to pay attention to where the actual stock is on the outside of the part.  Inside he part seems to work great, but outside, not so much.

 

I'm currently using a containment chain around the outside of the stock, but I've tried a manually defined region well outside that as well.  Exact same results: outside the part model it cleans out the entire containment region just like it's a pocket, ignoring the fact there is no stock there.

 

Please tell me I am missing something easy here? :-)   These are prototype runs, so the cycle time isn't a big deal yet, but I would really like to understand how to make this operate the way it's supposed to.

 

 

[BCW]

Make sure under "Toolpath Type" you have "From Outside" selected. I suspect right now it is set as inside.

[dvandewalle]

Make sure under "Toolpath Type" you have "From Outside" selected. I suspect right now it is set as inside.

Unfortunately is seems that when you have rest mode turned on, the inside/outside radio buttons get grayed out.

I've read on other forum threads that in rest mode, MC is supposed to always start from the outside if it has room between the containment region and the stock.  They problem is it doesn't seem to be doing that ...

[neurosis]

It will if you play with your containment settings.

 

Set your containment to Compensate to "outside" and add some extra offset to it and see what you get.

 

edit:  Scratch that - it looks like you've already done that.  How do you have your rest material defined?

[Müřlıń®]

You are using too big a offset....just offset .01 bigger than the stock left on the walls...

[BenK]

I reported this a few years ago. They changed the logic behind the chaining around the time X7 came out and ever since it hasn't worked correctly in my opinion. 

 

My question about what you're trying to do is, why are you using opti-rest? Just use the regular opti-rough using from the outside.

[BCW]

Unfortunately is seems that when you have rest mode turned on, the inside/outside radio buttons get grayed out.

I've read on other forum threads that in rest mode, MC is supposed to always start from the outside if it has room between the containment region and the stock.  They problem is it doesn't seem to be doing that ...

Ah, right. I guess I based my answer more on the picture and assuming you were optiroughing (my bad, it even stated optirest in the title lol). Usually when I do optirest roughing I will set my containment boundary much larger than the area to be milled and just let the computer do the work on analyzing whats leftover to cut. But in your instance it looks like you would be better off using optirough without a rest material since this is the first toolpath after facing, no need for rest material I would guess.

In this pic you can see the grey area is the stock I want to mill and the containment boundary far exceeds where my cutter needs to go.

[dvandewalle]

So I spent FAR too many hours at home last night jacking around with this.  Pretty much every piece of advice on this in this thread and that I've dug out of the archives is correct at one point or another. It's quite an interesting problem, I think I've actually located a bug in MCx9.   The behavior is very very inconsistent.

 

I made a really simple contrived example in a brand new project with an simple box buried in a chunk of stock.  I found that when I first generate an optirough for that part everything works just great - MC comes in from the outside at full depth for the profile roughing, without doing trochoidal, and helixes in for the pocket.  All good.  

 

Now when I flip on rest mode (because in real life I want to clean up certain surfaces with a face mill first) things get a little odd.  It no longer wants to come in from the outside, instead it ramps down into the stock around the periphery and then whips around the outside without going troichoidal.  No exactly what I wanted, but still reasonable.  I can understand how it go there.

 

Now for the kicker: if I turn rest mode back OFF, something got stuck!  It does not jump back to the way it was working before, but keeps the new style tool path.  At this point it's really really sensitive to the containment offset number.  If it gets too large, it jumps into full troichoidal, if it's small enough it stays with nice linear paths.

 

That's the part that is really freaking me out: I expect software to exhibit reversible behavior when I flip options on and off, not store some kind of behind the scenes sticky configuration ...

 

Hmmmm .... actually it looks like if I turn rest back OFF, then flip the type of path to "From outside", then turn rest back ON, it generates what I want.  It's like they didn't fully disable the selector button even though it's turned off!

 

Argh! :-)  Very inconsistent behavior.

[neurosis]

Can you take a screen shot of how you have your rest material set up?  Is it set to your stock model for "one other operation"? 

 

Ive had this problem with older part files when bringing them in to X8 or X9.  In the past you were able to use "from outside" with optirest.  Now that options is removed and when using a single operation (or all other operations) THAT WAS NOT A STOCK MODEL it would do exactly as you are showing in your photo.  I had to create stock models and use those as the "one other operation" and then I would get the results that I expected.

 

Can you share file that isn't working properly?

[crazy^millman]

So I spent FAR too many hours at home last night jacking around with this.  Pretty much every piece of advice on this in this thread and that I've dug out of the archives is correct at one point or another. It's quite an interesting problem, I think I've actually located a bug in MCx9.   The behavior is very very inconsistent.

 

I made a really simple contrived example in a brand new project with an simple box buried in a chunk of stock.  I found that when I first generate an optirough for that part everything works just great - MC comes in from the outside at full depth for the profile roughing, without doing trochoidal, and helixes in for the pocket.  All good.  

 

Now when I flip on rest mode (because in real life I want to clean up certain surfaces with a face mill first) things get a little odd.  It no longer wants to come in from the outside, instead it ramps down into the stock around the periphery and then whips around the outside without going troichoidal.  No exactly what I wanted, but still reasonable.  I can understand how it go there.

 

Now for the kicker: if I turn rest mode back OFF, something got stuck!  It does not jump back to the way it was working before, but keeps the new style tool path.  At this point it's really really sensitive to the containment offset number.  If it gets too large, it jumps into full troichoidal, if it's small enough it stays with nice linear paths.

 

That's the part that is really freaking me out: I expect software to exhibit reversible behavior when I flip options on and off, not store some kind of behind the scenes sticky configuration ...

 

Hmmmm .... actually it looks like if I turn rest back OFF, then flip the type of path to "From outside", then turn rest back ON, it generates what I want.  It's like they didn't fully disable the selector button even though it's turned off!

 

Argh! :-)  Very inconsistent behavior.

 

Copying operations and making changes to existing operations seem to cause this quite a bit. Best thing to do is to figure out what you really need. Once you do make a fresh operation set the correct way and go from there. Messing around in certain operations to tinker or dial them in seem to really give Mastercam a fit. Our team has noticed the bigger the file the more compound it gets.

[dvandewalle]

Can you take a screen shot of how you have your rest material set up?  Is it set to your stock model for "one other operation"? 

 

Ive had this problem with older part files when bringing them in to X8 or X9.  In the past you were able to use "from outside" with optirest.  Now that options is removed and when using a single operation (or all other operations) THAT WAS NOT A STOCK MODEL it would do exactly as you are showing in your photo.  I had to create stock models and use those as the "one other operation" and then I would get the results that I expected.

 

Can you share file that isn't working properly?

 

I had not tried setting the stock model to a manually defined intermediate for just "one other operation";  that works!  Just a simple box stock definition and it's all good - x9 generates a gorgeous high-speed/low-drag tool path that is exactly what I wanted. 

 

It really really sucks that we have to do that - it kills the speed of a workflow and makes what should have been a really nice toolpath type more of a pain in the arse to utilize.  It just acts like it doesn't know where the stock is anymore, when I damn well know that it does!

 

I'm used to CAM that is a lot more "stock aware" between operations ... the learning curve on x9 is turning out to be kind of harsh.

 

Thanks for the workaround, I owe you a beer!

[neurosis]

 

Thanks for the workaround, I owe you a beer!

 

 

No problem.  I have probably 50 part files that were created back when we were able to use "from outside" on opti-rest.  Any time I open one of them and have to regenerate, I end up having to make all of these changes to bring them up to date.  Now THAT is frustrating.  

 

Glad that you were able to get the results that you were looking for.

[kunfuzed]

I've also noticed this.  I've been successful with "outside" like you have it set, and then set my "offset" to 50% of the cutter diameter.

[SpacePilotPro]

I have also found this same problem when opening an X7 file with X9 and regenerating the opti-core toolpath. It will switch to containment inside, even though all the parameters say it should be outside. I have found no way to fix it aside from creating a new toolpath. It is indeed frustrating.

[jlw™]

Thought you guys might enjoy this:

 

[mike93]

• some times i think this is the problem
•  
•  
•  
• Front page
• Main blog
• Machining blog
• goatchurch

 

Freesteel Blog » Steel cutting of shapes

Steel cutting of shapes

Monday, January 25th, 2016 at 1:42 pm Written by: Julian

Here’s a quick offering from the “Well it’s better than nothing video editing department”. This is the result of 2 days of cutting from short videos taken with my camera. (I’ve got no talent with video editing.)

I learnt one heck of a lot in the process.

1. Steel is really difficult to work with

Small 3mm cutters are easy to snap

The spindle is under-powered

Big 6mm cutters can handle being bent when the spindle stalls if you hit stop soon enough

You can drop the feedrate briefly to stop the spindle stalling

Multiple cutters with rest machining are essential

0.1mm stepovers are a better than 0.2mm

I probably need a tapered cutter to create a draft angle

Clamps are a real hassle; I’m going to get a vice

The noise of the machine sounds terrible, but nobody has complained yet because it doesn’t seem to carry into the hallway

My 3D printed ductwork for automatically hoovering out the chips was a failure; I need to prod in the nozzle by hand to remove the chips

I was using the Adaptive Clearing toolpaths in Autodesk Fusion, which I had spent 10 years developing before and after it got sold to AD.

It sucked in several ways that I did not know about, because I’d never used it myself to get something I wanted to get done. I always said I ought to have been put on the job of using CAM software to cut steel on a machine in a factory for a couple of months at some point in my career before being allowed to continue writing software that didn’t quite do stuff right. People get into positions like I was, and seem to do pretty well, but should get the opportunity to go back and fill in some gaping holes in their experience.

The problems I found were:

1) Adaptive takes too long time to calculate small stepovers when clearing around a tongue of material and it has to turn right towards the material to stay in contact. This is probably because the sample rate has to go very small in order to maintain engagement when it does its straight line forward samples. It should detect these situations and do its initial step forward with a curve to the right so that begins with being engaged on the first sample and doesn’t need to resample backwards blindly until it makes contact again.

2) The helix ramp down pitch was not linked to the tiny stepover I was setting and I couldn’t see how to change it. I had to hack the G-code directly.

3) In spite of claims to the contrary and it being mathematically accurate, I am sure that the load going into the corners is higher than when the flank cutting is on the straight. I can hear the spindle being slowed down. This could be because the chip length is longer for the same chip width. The chip length is the distance around the circumference of the cutter that is tearing off the metal, and it can approach a semicircle in a tight corner, or be insignificant when it first engages with the 90degree outer corner of the stock.

Now a real machine tool probably has so much angular momentum in the spindle that no one is going to notice this, but on some underpowered low-spec experimental device, such as this, it becomes apparent. That’s why future innovations would happen here, and are unlikely on the big machines where you don’t notice the flaws.

I can now pretty much see how companies like IBM missed the first wave of the PC, which were toy devices in comparison to the big mainframes they were playing with. Nobody was ever going to do any real work on those barely-up-to-scratch microcontroller-based computers with deplorable amounts of RAM, audio cassette tapes for backup, a complete joke parody of an operating system from Microsoft, and a lack of customers able to pay big bucks. Most of the professional engineers in the world (software and hardware) had all the access they needed to mainframe computers in their workplace or university institutions to do fluid dynamics or graphics or simulations. I’m sure when some overly keen teenager came along with their toy machine he’d soldered together, they put him in his place with a back-of-the-envelope calculation of how many centuries it would take that Apple2 to do something real, like predict tomorrow’s weather, which was something they could do with their latest cool CrayXMP super-computer machines. PCs were obviously an utter waste of time, and because was clear where the cutting edge was if you wanted to actually get stuff done.

Sure, you could say this left a huge gap in the economy for new tech billionaires to emerge and for IBM to eventually become an embarrassment, but think about the wasted capital and precious engineering time of talented people who should have been deployed to make this microcomputer tech good from the beginning. MS/DOS and MSWord might not have existed in the horrible no-good forms they did had it not been left only to people who didn’t know what they were doing and had to learn as they went along, thus locked in their anti-productive design mistakes into the way this tech worked for the next 30 years.

Meanwhile I’ve no idea what I am doing. Should I spray WD-40 onto the metal while it is cutting?

Monday, January 25th, 2016 Written by: Julian Adaptive, Machining Trackback URL for this entry

1 Comment

• 1. Greg H. replies at 26th January 2016, 1:00 pm :

  You took the words from my mouth. I have been posting on the HSMWorks forum for a long time that development should run machines with the code they develop. Or development should hire seasoned machinists to run the code. Relying on customer feed back is the lazy way out and not very productive.

  As for coolant you want a coolant that is for cutting steel. WD-40 is OK for non-ferrous materials like alum, brass, copper. It is better than nothing at all on steel. I’m sure there is a machine shop near by, they will loan you some for the steel. Your machine seems a bit flimsy.

  Have a good one!

[mkd]

mike93,

 hey maybe just post a link (and a little snippet of the text) and add your comment below it, rather than doing a full text paste.

once pasted into your reply, if you highlight the text then click the yellow quote button, it will look better for us

[mike93]

i will try that next time, thank you.

[Redfire427]

You have a number of errors that will make this far more difficult than it needs to be. Your facing operations make no difference at all. Just do a dynamic roughing toolpath and choose a boundary that is the shape of the stock. You do not need to use "offset". Mastercam already knows to start from the outside. Another error I see in your settings is that your step-down is set to 1.2", but you also have step-up set at 1.2". This is totally useless based on your settings. Shut it off if all your surfaces are vertical. If your geometry is tapered, then set it to something reasonable that will give you some resolution. If you truly want to use a optirest roughing toolpath, it really doesn't need a boundary. Mastercam will calculate its own boundaries where it determines that stock still remains from a previous operation/s. If you truly want to only clean up a certain area, then that is where boundaries come into play. Don't blame the software for not giving you want you want. Your programming approach is incorrect. 

 

Carmen

[dvandewalle]

 

 

You have a number of errors that will make this far more difficult than it needs to be. 

That's totally possible!  I don't allege to have mastered this thing yet ... I have been using other CAM systems for a long time though; this is not my first rodeo :-)  

 

However ...

 

 

 

Your facing operations make no difference at all. Just do a dynamic roughing toolpath and choose a boundary that is the shape of the stock. You do not need to use "offset". Mastercam already knows to start from the outside. 

This is not really relevant and certainly is not an error. The CAM package doesn't get to pick my machining strategy for me.  Could I let it just rough that first, yep.  Do I want to in this case?  Nope.  I actually want to face that to start with and I have a reason for that.  The program is supposed to handle rest machining - it should cope with whatever I want to do first and calculate the remaining stock.

 

 

 

 You do not need to use "offset". Mastercam already knows to start from the outside.

 

It seems that if you don't manually define a new stock model for optirough type operations you DO need to use offset, or it doesn't start from the outside.  If you do create a new stock model (which it seems you pretty much have to) AND separately create a larger containment boundary than the stock, then yeah, you don't need the offset.  If you use a chain around the stock as the containment you NEED the offset or the tool won't leave the outer bounds where you have less stock than the tool diameter.  That's what it's for, it works fine.

 

 

 

Another error I see in your settings is that your step-down is set to 1.2", but you also have step-up set at 1.2". This is totally useless based on your settings. Shut it off if all your surfaces are vertical. If your geometry is tapered, then set it to something reasonable that will give you some resolution.

So, what's the correct way to get the system to generate a single full allowed depth cut in one op without defining the cut as a step up?  I'll tell you step down on it's own with a depth set to do the outside in one shot sure doesn't do it - it generates only outside cuts and no operations on the pocket.  If you don't tell it to step up, it won't pocket the center of the part and do the outside roughing to different depths.  I know what step up is intended to actually do and I agree 100% it should work the way you say - problem is that it doesn't generate what I want, which is single depth paths.   If there is a better way to rough this in one op than the settings I'm using please share!

 

. 

 If you truly want to use a optirest roughing toolpath, it really doesn't need a boundary. Mastercam will calculate its own boundaries where it determines that stock still remains from a previous operation/s

 

Yeah, that's exactly how it should work and how every other rest capable CAM I've used worsk.  Problem is that it doesn't actually work all the time here.  Sure, some operations calculate remaining stock just fine - OptiRest seems to not be one of them.  Sometimes it works, sometimes it doesn't.  Try generating an optirest  without defining containment -  you get a neat little dialog box that says: "A containment boundary is required for rest roughing."  Will it auto-generate one, yeah, but if you don't put an offset on the auto-generated version it won't work in all situations because it follows the drive surfaces for the limits, not the stock.

 

I absolutely blame the software for some of this and here's why: I made a simplified test case that worked great (same sizes, less complex internal geometry.)  I messed with it a little and it STOPPED WORKING with the same settings that I started with.  That's a software problem for sure.  I took the same settings that work on the simplified test case and applied them to my real part with freshly created operation - and they don't work.  To me that's a software problem as well (or just truly massive ignorance on my part, which is always a possibility. :-)  

 

To me rest machining means that the software should calculate the REmaining STock and target it for removal.  MCx9  doesn't seem to reliably do that. I don't understand why as I know it CAN reliably create a very good stock model from a list of operations.  If I create a stock model from prior ops (as opposed to defining a box stock) optirest sometimes works and sometimes doesn't.  If I create a box stock, it seems to work like a champ every single time.

 

I don't consider having to manually define a stock model each time I want to use optirough to be actual rest machining.  This part is being run on a 5-axis machine as a 3+2 and I have 5 different optirest operations defined right now.  Three of them turned out to require me manually defining a new stock model to get them working.  Two of them didn't (and these were ops well down the list) - it just worked out of the box like it you say it's supposed to. Same exact settings, just a different plane.  It SHOULD work ALL the time!

 

[BenK]

That's totally possible!  I don't allege to have mastered this thing yet ... I have been using other CAM systems for a long time though; this is not my first rodeo :-)  

 

Your experience with other software is irreverent, are you using the tool at hand correctly? I would say no.

 

 

This is not really relevant and certainly is not an error. The CAM package doesn't get to pick my machining strategy for me.  Could I let it just rough that first, yep.  Do I want to in this case?  Nope.  I actually want to face that to start with and I have a reason for that.  The program is supposed to handle rest machining - it should cope with whatever I want to do first and calculate the remaining stock.

 

Your facing operation is in fact of no concern for your roughing. All you need to do is set your steep/shallow to the correct depths. So you can face the part first than have the roughing come next without using a rest toolpath. The toolpath isn't design to handle "whatever you want it to do" it is designed for you to get a type of output based off of user input. In this case you are using it incorrectly. 

 

Don't blame your lack of understanding on the software. You asked for our help but when we point out what your issue is you are getting defensive and telling us we are wrong. Not exactly the way to get people to help you is it? If you would like, post up a file and we can show you the correct way to accomplish what you're after. If you go into it with an open mind you might just learn something.

[dvandewalle]

Sorry if I'm coming across as defensive, that's just frustration speaking.  I am extremely open minded - if it works I'll use it.  I just like to understand the why.  Defining a new box stock around the area to Optirough seems to work, and I'll happily continue to use that to get work done.

 

I guess this program just has a very different paradigm for where rest machining is appropriate.  It seems like things are more predictable when avoiding it when possible instead of reaching for it first.  I suppose that's the lesson I need to take away from this.

 

Edit: Just to be 100% clear - I'm very grateful for this forum and any help that's been offered.  It's been incredibly helpful in learning Mastercam.  I can't imagine having to learn this thing without being to read though all of these posts. 

[Redfire427]

Your replies to my comments are certainly defensive.

 

You are attempting to use the toolpath incorrectly. It is not designed to be used the way you intend. Go back and re-read my comments. 

 

Face the part,no problem, who cares. That part makes sense and would be a typical approach to roughing this part. As BenK graciously suggested, use the depth limits to control where your follow-up toolpath cuts. 

 

Again, step-up is only valid where you have surfaces/solids that have topography that is between flat and vertical. By the looks of your model, you have vertical walls and flat floors. Step-up would have no value here as there is no material left behind at each profile pass. You need sloping surface/solid faces for step-up to have any use.

 

I think the part you are not understanding is: You are not using the correct toolpath to rough this part. Basically, if you complained that you are using a waterline toolpath and the stupid software doesn't pocket out all the material. I would tell you the same thing. Use the appropriate toolpaths correctly and you will get the correct results. In your example, you are pushing on a rope. It doesn't work that way.

 

Carmen