HST Waterline not working right

[Bob W.]

I set up a waterline toolpath to machine from 2 degrees to 90 degrees and it is only machining a fraction of the geometry (picture below). Is there something I am doing wrong here? It seems that every time I go to use these toolpaths I spend more time trying to get them to work right than if I just used the old surfacing toolpaths. I ran into the exact same issue on horizontal HST where it only machined a fraction of the actual horizontal regions. I REALLY, REALLY, REALLY wish CNC software would invest the time to get these to work right, or invest the time to improve the old surfacing toolpaths to make them more efficient. For something that is supposed to make my job easier these HST toolpaths end up wasting a ton of my time. If there is a way to get these working right maybe CNC could release the guide "The Black Magic Guide to Getting HST Toolpaths to Work Properly". They would probably make some serious $$$ on that publication.

 

According to Mastercam this finishing operation should take ~3 HST toolpaths, Waterline, Horizontal, and either raster or scallop. It just NEVER seems to work that way and it is going to make for a really long Sunday...

[NOTW Programmer]

POst the MCX so I can take a crack at it and reprogram it for you then you can determine if its worth it or not. HST usually saves me tons of time up to 5 times less while roughing a part.

[Bob W.]

I can't post this file unfortunately. Any idea why it is missing the bosses and rib features? I do all of my roughing with Volumill and that package is fantastic.

[Newbeeee™]

... maybe CNC could release the guide "The Black Magic Guide to Getting HST Toolpaths to Work Properly". They would probably make some serious $$$ on that publication.

 

 

Sorry Bob. Can't help with the toolpath.

But I would buy the book

[gcode]

If I were doing that toolpath I'd set it to 0 to 90° and use depth limits to keep it off the floor

[MotorCityMinion]

Make sure your not using a bull nose EM on the Horizontal path as well. I think that having to use a sharp cornered EM on the floors is ignorant but the fact remains that this tool path is buggy with bull mills.

 

Why the waterline path isn't machining those other bosses, IDK. Did you select the whole model? Using boundaries by any chance?

[gcode]

Make sure your not using a bull nose EM on the Horizontal path as well. I think that having to use a sharp cornered EM on the floors is ignorant but the fact remains that this tool path is buggy with bull mills.

 

Why the waterline path isn't machining those other bosses, IDK. Did you select the whole model? Using boundaries by any chance?

 

 

I ran a wicked part in X6 beta last moth using a lot of high speed paths

 

I used a bunch of Horizontal finish paths using a Ø1 x .12R insert mill and it worked very well

plus bunch of rest rough using STL's as stock and one of the hybrid rest roughs that was a really sweet toolpath.

 

My first attempt at hybrid rest rough had a really bad gouge in it, but fortunately I found it via backplot

instead of real life on the $7K piece of aluminum I was cutting.

[Bob W.]

If I were doing that toolpath I'd set it to 0 to 90° and use depth limits to keep it off the floor

 

The floor isn't flat unfortunately. It has a very slight drop in Z and it also has a bit of curvature.

 

Why the waterline path isn't machining those other bosses, IDK. Did you select the whole model? Using boundaries by any chance?

 

I selected the whole model and used boundary chains to keep it from going outside the extents of the model to protect the fixture. The boundary chain is visible in the picture above as a grey curve.

[gcode]

did you try 0 to 90 with the floor as a check surface

[88Matt]

If I were doing that toolpath I'd set it to 0 to 90° and use depth limits to keep it off the floor

I do this all the time.

[Colin Gilchrist]

Hi Bob,

 

Can you send this one into QC? I'd like to test this in X6 if possible. We've made a bunch of enhancements to the HST Toolpaths. One Enhancement that will be of particular interest to you and other HST users is the new Check Surface Support. In the previous versions of Mastercam (X5 and below), the HST Toolpaths treat Check Surfaces as additional Drive Surfaces. The Toolpath has been refined to include real Check Surface support (basically the HST paths will now treat the Check/Drive regions more like the legacy Surface Toolpaths did. Areas that need to be cut, and areas that the tool needs to stay away from).

 

How large is the file? If necessary I can give you an FTP Site (not the one listed here) that you can use to upload the file for QC.

 

Thanks,

[peon]

That happens to me once in a great while on 90° walls and I haven't found a fix. You can try toolpathing with Surface Finish Contour, but that rarely fixes the issue. Like I said, I rarely see this issue to begin with. Set your "Skip pockets smaller than" to "0" on the "Transitions" page and see what happens.

[Redfire427]

Bob,

 

Please don't confuse the toolpaths not working, versus, not knowing how to use them. The HST toolpaths work perfectly when used correctly. If you are not getting the results you expect, then you simply are not using the toolpaths correctly. There is ALWAYS a reason why. It could be any number of things. It could be the size of tool and corner radius you have selected, boundaries, depth limits, "Skip pockets smaller than", lead-ins/outs,corner rounding, etc, etc.

 

There was a comment above regarding horizontal. Bullnose endmills work perfectly for these toolpaths. There is no need at all to program a sharp cornered tool.

 

Learn to use them.............you will then love them. Just train yourself to completely forget about the old "legacy" toolpaths. They are total junk compared to the HST toolpaths.

 

Carmen

[MotorCityMinion]

"There was a comment above regarding horizontal. Bullnose endmills work perfectly for these toolpaths. There is no need at all to program a sharp cornered tool."

 

Perhaps this is the case in X5, but in previous versions, I know for a fact that in some cases I had to set a ridiculously low step over percentage in order to not leave cusps or bumps on a flat surface. Usually this occurred when using containment boundaries to avoid bolt heads. Others have stated their problems with bull nose emills not cleaning up as well. When I select a surface with no boundaries, I get a nice tool path with a bull nose Em.

[Chris Rizzo]

then you simply are not using the toolpaths correctly. There is ALWAYS a reason why.

 

A bit harsh, because sometime the reason is a bug. Are you driving surfaces or solids? Try driving just surfaces if not already. Also check your PM.

[Bob W.]

That happens to me once in a great while on 90° walls and I haven't found a fix. You can try toolpathing with Surface Finish Contour, but that rarely fixes the issue. Like I said, I rarely see this issue to begin with. Set your "Skip pockets smaller than" to "0" on the "Transitions" page and see what happens.

 

Well, Peon nailed it. Modifying this setting fixed the issue, even though there were no pockets :-). Maybe the wording on that setting could be revised. I might have been a bit quick to point fingers as well but given the history of issues I have had with the HST it is understandable. These issues include gouging, retracting with the ball mill tangent to a vertical wall creating marks, retracting with the tool tangent to the part surface when it should be .15" above, etc... These are anything but bulletproof and it typically takes 3-5 tries when things are going smoothly. Ultimately I did get the part finished with my three HST toolpaths but it was anything but smooth getting there.

[neurosis]

"There was a comment above regarding horizontal. Bullnose endmills work perfectly for these toolpaths. There is no need at all to program a sharp cornered tool."

 

Perhaps this is the case in X5, but in previous versions, I know for a fact that in some cases I had to set a ridiculously low step over percentage in order to not leave cusps or bumps on a flat surface. Usually this occurred when using containment boundaries to avoid bolt heads. Others have stated their problems with bull nose emills not cleaning up as well. When I select a surface with no boundaries, I get a nice tool path with a bull nose Em.

 

 

I'll back this up.. Ive seen it several times myself. RIDICULOUSLY small step overs in order to alleviate cusps.

[Thee Rickster ™]

small step overs in order to alleviate cusps.

 

Try using add cut?

[neurosis]

Try using add cut?

 

 

I am talking about Horizontal surfaces. (I assume Motor is too).

 

 

Make sure your not using a bull nose EM on the Horizontal path as well. I think that having to use a sharp cornered EM on the floors is ignorant but the fact remains that this tool path is buggy with bull mills.

 

Why the waterline path isn't machining those other bosses, IDK. Did you select the whole model? Using boundaries by any chance?

 

 

Ive actually went as far as to manually add cuts to remove cusps on the horizontal path so that I didnt have to use such a horribly inefficient tool path by reducing the step over enough to clean the cusps.

[peon]

Yep Bob, the software has a tendency, now and then, to identify islands and small cores as a pocket. You'll see this more often when you have to program trodes. You have legitimate complaints about the HST's and you have to play with some of the parameters to get what you want. To avoid your retract issue, NEVER use the "Minimum Distance" as a retract method. I almost always use "Minimum Vertical Retract" with "Output feed move" checked and set the feed parameter to your highest feed rate. Or, use "Full Vertical Retract" on the slower machines. These 2 methods won't drag the tool over the top of the steel causing a gouge. On Waterline toolpaths, I enter a zero value in "Vertical arc entry/exit" leads. In most cases, that is totally unnecessary and will certainly dog on older machine and slow down a fast machine. Once you figure these little tricks, you will use the HST's for most of your surface machining.

[Redfire427]

Well, Peon nailed it. Modifying this setting fixed the issue, even though there were no pockets :-). Maybe the wording on that setting could be revised. I might have been a bit quick to point fingers as well but given the history of issues I have had with the HST it is understandable. These issues include gouging, retracting with the ball mill tangent to a vertical wall creating marks, retracting with the tool tangent to the part surface when it should be .15" above, etc... These are anything but bulletproof and it typically takes 3-5 tries when things are going smoothly. Ultimately I did get the part finished with my three HST toolpaths but it was anything but smooth getting there.

 

 

I would like to clarify my position on my comments posted above. I use the HST toolpaths almost exclusively because they are designed for high speed machining which I do everyday, so needless to say, if the toolpaths didn't work properly............I would know. When I use HST horizontal with a bull nose endmill, I typically use 40% as my stepover to prevent the cusps issue that was mentioned. I'm not saying this is good, but it works just fine. Mastercam has had the same issue even with the "pocket" toolpath leaving cusps since version 3 ( not X3, but rather Version 3, yeah, I've been around for a while ) The size of rad on the endmill will dictate the step-over as the larger the corner radius is, the smaller the flat area is on the tool. I have used the HST toolpaths since they came out so many years ago. I have not had one single gouge in all these years. I do most of my programming using surfaces rather than solids.

 

If you do not use the toolpaths correctly, then you will get poor results. The same can be said for the legacy toolpaths. If you input garbage, then you will get poor results. Bob, I urge you to learn what each function does and apply it accordingly, rather than make accusations about the software not working properly.

 

Carmen

[MotorCityMinion]

"Bob, I urge you to learn what each function does and apply it accordingly, rather than make accusations about the software not working properly.'

 

Bob had his underwear in a bunch that day and we've all been there. Still, 40% step over? Works just fine? 40% might be fine for a one off or a hairy situation, but not in a multi part run. I always calculate step overs for a floor based on the cutter diameter (minus the rad x 2 ) x .70 then tweak accordingly if I can reduce a few passes.

[Bob W.]

If you do not use the toolpaths correctly, then you will get poor results. The same can be said for the legacy toolpaths. If you input garbage, then you will get poor results. Bob, I urge you to learn what each function does and apply it accordingly, rather than make accusations about the software not working properly.

 

You have a point, I am not an expert on the HST toolpaths but with what Peon and others have said, and what I have experienced, there is more than just knowing what the settings do. There is a little tribal knowledge that goes along with getting these toolpaths to output good results and that's what is frustrating. Having the 'ignore pockets' setting too large caused the waterline to skip several bosses and ribs. Well, bosses and ribs aren't pockets... The issues with the retract strategy and gouging is a real one. I also had a hybrid toolpath violate the containment boundary by 1.5" the other day and gouge the part. What setting did I miss there? I typically use the minimum distance retract strategy and I have had the tool tip dragged across the top of my part at Z=0.000 leaving a mark. Is that supposed to happen when my part clearances are set to .1"? There is a lot more than just knowing what the settings do in getting these to work right and that is what Mastercam needs to work on. It makes it difficult for one that uses the toolpath sporadically and doesn't have the tribal knowledge down. It sounds like what I really need to learn is what settings to watch out for because they don't quite work how they are supposed to.

 

Bob

[Watcher]

+10000000

[Newbeeee™]

Peon/Carmen,

Perhaps you two should get together and write "The Black Magic Guide to Getting HST Toolpaths to Work Properly" that Bob was asking for in post 1

As I said, I'd buy a copy from you.