Surface Finish Anger

[Rocketmachinist]

I have been trying to get a finishing path to work on a round part I'm doing. I want to get waterline to work but every time I get an error saying that something is invalid or it just takes way to long to compute. Anybody have any tricks to get waterline to work with a good finish, and not drive me crazy in the process?

[Guest]

Well, I can not possibly tell you if a waterline will work without seeing what you're trying to cut.

[delete]

Well, I can not possibly tell you if a waterline will work without seeing what you're trying to cut.

WATERLINE

It needs TWO Boundries sometimes Inside and an outside cut in between the two .and then play with the tool / center / offset blah , blah ...

She'll crunch the numbers...Also I don't use the new smoothing filter because it add's another go round of number crunching.

(It does work well though)

Also I have never had any luck with the Check surface option only Boundries.

(Even though it's there for you to pick)?

To save even more time I first plug in a .100 z cut depth etc. so I don't burn the clock as I am seeing if

Waterline is even going to do what I wanted.

 

THE TOOLPATH ROCKS ! Just takes some "Mastery"

[Guest]

you're thinking of a Surface Finish Blend needing 2 boundaries and it cuts between them

[MotorCityMinion]

Yup, just select the part as boundaries are not a requirement for waterline or SF contour if your machining around the entire part. Start with no filter and a step down around .05. Do not limit your depths at first either. Those 2 tool paths always pop quickly when the defaults are not monkey'd with.

 

All tool paths suck? They sure do, until you learn how to use them correctly.  Been there as well. I still have several sucky tool paths stumping me.     Have a few cold ones, put on some headphones and try it again.

[Mcam Nut]

Have you tried hybrid? Seems to work great

[Redfire427]

These types of errors are usually caused by the hardware in front of the keyboard, rather than behind it. Go through your toolpath and look at each value you have imput. You must be asking Mastercam to calculate something that is not possible. Check to make sure your WCS/Toolplane are correct. Also, make sure you do have "add cuts" checked unless you know how/where to use this function. This one function will add tremendous calculation time to your processing. I calculate waterline toolpaths on thousands of surfaces in seconds every day without issue, mind you, my computer is also up to date hardware-wise, infornt of the keyboard, and behind it.

 

Carmen

[Tyler Robertson]

This is a post I take exception to - if there's one thing Mastercam does well is gives a number of different ways to do a part: and there's always a way to do it.

Is waterline the best path for what you're doing? can you post a part?

 

go back to your default values - does it work?

Set a Large stepover - let that calculate. Do you see odd tool motion? Check different options in the path using a large tolerance/stepover

 

if a toolpath isn't calculating, pull it back. Let it calculate based on large stpeovers, large tolerances so you can at least see what's going on. get the toolpath right, and then crank up the tolerances/stepovers.

Sometimes these will introduce errors with some features, but most of the time they'll react in a straightforward fashion

[Bob W.]

To speed things up I set the step down pretty coarse ans I also set the tolerance to .005 - .010. Once the toolpath looks good I set the tolerance and step down at their final values. I have tried the hybrid toolpath a few times but it rarely works. Not sure why, but I get 'unable to find valid machining zone' errors so I have given up on it. It only worked ~30% of the time and I was able to get better results with the other toolpaths anyways.

[Richard Thomas - Mastercam UK]

And check your Tool/Construction planes!

[KMartin]

Try using a smaller tool .

 

MasterCam X5

Mill Level 3/Solids - Moldplus

Intel 5150 2.66GHz, 2.0 GB RAM

Windows XP Pro SP3

NVIDIA Quadro FX 3450

[LaszloK]

I guess I have to take exception with suggesting a different toolpath when one does not work. Although waterline might not be the "best" solution, it should still function properly and produce a toolpath for any part. Other's have posted good suggestions like big stepover and tolerance, minimum depth, and just running with defaults at first. One way to determine the "best" solution is to experiment with several methods. This can be difficult when some toolpaths are difficult to work with.

[Guest]

I still fail to see how any of us can tell him what's wrong when we don't know what he's trying to do?

 

His posting pretty well makes me think he doesn't know how to use the path so he may or may not even be applying it to geometry in which it is suited to cut.

 

JM2C

[LaszloK]

I agree John, that seeing the part would help with suggestions to make waterline work. That was the real issue and solutions should not be to abandon the toolapth and try something else. A different toolpath suggestion could get the job done better, but would not help with the initial problem.

[Mr. Wizzard]

Like almost everyone has said, it's hard to offer advice with very limited information. I'm sure you would get some help ASAP with a better description of the problem, or even a picture. Most of the time a toolpath won't work for me because i've done something stupid and didn't notice it. The only time I really get frustrated is when I set up a surface toolpath, let it chug along calculating, and end up getting an error that cancels all progress.... In these instances, I use the help menu to see if I have set some parameters incorrectly. If you can't figure it out, try another toolpath. There's usually many different ways to get the desired result. If you say the toolpath sucks, it very well may suck. But it might suck because it is being applied incorrectly or not be designed for the specific thing you are trying to make it do.

More information will definitely get you in the right direction, but just saying the toolpaths suck won't help you out.

[Rocketmachinist]

Thanks everybody,

 

I was trying to get a good surface finish on my part and had a .002 stepover on my part. Not only would it take forever to process most of the time Mastercam would crash. I went with contour and the same thing. I kicked my tolerances back to .005 and it started working great. I just need to remember to try and do a very large tolerance first and forwards from there. It just gets a little frustrating when your toolpath errors out and all that it tells you is to call your reseller.

[Mr. Wizzard]

Been there, done that 100 times. It does get very irritating when it kicks you out and does not tell you why. Like you already figured out, it's good practice to first try a finishing pass with a way high stepover and see if it will even accept it. Then, when you have the parameters correct, you can "smallerize" your moves for a good finish and let it work.

Good luck to you.

[delete]

There have been times I had to make two boundries one at the top of a cone shape that had a flat on it

(So it wouldn't gone down in it) and one at the base or the toolpath because it wouldn't go down to the bottom

Even with a a Z number called out, etc. It was the only way it would cut all of it !?!.

[Tyler Robertson]

Thanks everybody,

 

I was trying to get a good surface finish on my part and had a .002 stepover on my part. Not only would it take forever to process most of the time Mastercam would crash. I went with contour and the same thing. I kicked my tolerances back to .005 and it started working great. I just need to remember to try and do a very large tolerance first and forwards from there. It just gets a little frustrating when your toolpath errors out and all that it tells you is to call your reseller.

 

If this is the case, there may be memory settings on your computer/windows/mastercam (configuration tolerances) that you can set so it won't crash on a part.

 

I just processed a 0.005" stepover on my laptop on a pretty big part with multiaxis calculation as well. If mastercam is crashing due a tolerance - there's something that can be done to fix it. In this case I WOULD check with your reseller to see if they can help you tweak your tolerances to get better results!

 

What's your computer system like? $100 in ram/processing power can be be easily worth it.

[Tyler Robertson]

I guess I have to take exception with suggesting a different toolpath when one does not work. Although waterline might not be the "best" solution, it should still function properly and produce a toolpath for any part.

 

Any part? There's an infinite number of different ways a part can be designed badly for maching - some toolpaths, based on how they calculate motion, can be better at handling situations than others. Some paths use containment bounderies while others don't. Some paths use additional calculation to add 'intelligent' depth cutting etc.

 

Take Flowline 5-axis. This toolpath has been around for eons - It can calculate on multiple surfaces... IF those surfaces don't have changing flowline directions: as soon as that happens you can't get it to calculate - gives a Flowline error. You have to re-create your geometry as one surface, OR

 

Use Advanced Multiaxis and it'll create the path

[LaszloK]

Any part that is modelled correctly, yes. Again, there could be better paths to use but the waterline path should work also. If the response is to use another path, then why even offer waterline?

[Ocean Lacky™]

Any part that is modelled correctly

 

Yes! But what to do if a part is flawed? Anytime I get a model that takes an unusually long time to generate a toolpath, Analyze/ Test Surffaces is my friend. Even the smallest surface where the Surface Normal suddenly changes direction can send Mastercam into shock.

[Tyler Robertson]

Any part that is modelled correctly, yes. Again, there could be better paths to use but the waterline path should work also. If the response is to use another path, then why even offer waterline?

 

I don't know if the part is modeled correctly - there's no empirical evidenece that waterline just doesn't "work" - But would you rather sit there and bang your head against the wall, or see if another path will calculate? If another path calculates then maybe you can determine root cause of failure with waterline.

The response is to use another path to see if you can get it done, and determine if the problem lies elsewhere - Toolpaths don't all calculate in the same fashion...

[LaszloK]

Any part properly modelled, yes. There probably is a better path to use, but if the response for providing help on the waterline path is to use another path, then why offer the water line path?

[Roger Peterson]

Toolpath choice starts at topology (steep walls, mostly flat flowing surfaces, combo, runner, etc...), and then other factors come into play. There can be an ideal toolpath for sets of surfaces, but many times toolpath choice comes down to personal preference based on experience, tooling, machine tool, etc... Three experienced programmers may approach the same part differently.

 

One persons idea of modeled correctly is another mans "What the **** is wrong with you", mastercam will cut either.