surface finish leftover

[TERRYH]

We typically use the surface finish constant scallop to finish most not all of our parts, say we use a 1" ball then for the smaller corners we use say a 1/2" ball what tolerances do you guys use in this situation we typically use .0005 to .001 and I know the larger the tolerance the less it will actually do. I done this on a recent part and did the left over from 1" to 1/2" then a 1/4" balls, the 1/2 did a great job yet the 1/4" did some funky wavy cuts and jumped all over the place in areas it really should not have been looking at. Kind of confusing when we use the same process over and over and it does well one time and crap the next with the same settings.

[Chris In-House Solutions]

Terryh is it possible for you to post the file you are talking about.  One of the guys here might be able to take a quick look and assist you with your settings to make the toolpath do what you are looking for.

[Guest]

11 minutes ago, TERRYH said:

We typically use the surface finish constant scallop to finish most not all of our parts, say we use a 1" ball then for the smaller corners we use say a 1/2" ball what tolerances do you guys use in this situation we typically use .0005 to .001 and I know the larger the tolerance the less it will actually do. I done this on a recent part and did the left over from 1" to 1/2" then a 1/4" balls, the 1/2 did a great job yet the 1/4" did some funky wavy cuts and jumped all over the place in areas it really should not have been looking at. Kind of confusing when we use the same process over and over and it does well one time and crap the next with the same settings.

It's not the same process Terry, your geometry has changed

As happens so often on the forum as late, sight unseen, it is tough to doing anything more than speculate on the exact reason for the issue you see,,,,

 

 

 

[TERRYH]

Chris I am not sure on the process to go thru to post this part, or if I even could being our I.T. dept has the net locked up pretty tight around here, lucky we can get on here. My biggest questions are why did the 1/2" run fine and look good with the same tolerance settings as I used for the 1/4"  using the same surfaces. And second going from the 1/2 to the 1/4 why was the 1/4 even looking at radii the 1/2 should have finished.

[crazy^millman]

Terry the only think I can think of is the basic idea of the 2 tools are not the same and they produce 2 different results. I through together this quick example. I did have to use 100X scale to get the dimensions to work and then use .001 scale in the dimensions to get the scaled output I wanted, but this should give you an idea. As the shape changes the 1/4 tool cusp height will vary a lot more and we expect see that increases on our cusp height.  On a flat surface changes the step over stays the same, but not the contact point of the tool as the tangential intersection of the tool comes in contact with the surface as it changes. Having done all of this for many years by hand I just get why there is the difference you are seeing. Not sure make cross sections of the areas and then make the same step over and project to that surface. then put the tools in contact with the tangential intersection of the tools at the tool contact point and then it should make more sense. It seems the software is acting wrong, but depending on the shape of the part it is doing what I would expect it to do. All thing equal this is not equal it this proportional, but that proportion doesn't stay the same when the shape changes. 

In the picture attached for the file linked I have taken and drawn a 1.000, .500 and .250 Ball endmill. I have stepped them all over .01 to scale the scale is 100X. You can see the cusp height changes to double then 4 times as each tool changes for the same step over. Now in irregular shapes this does stay the same. It can changes, because where the tool comes int contact with the surface will very greatly. That is where the math comes in and the algorithms take what was weeks of trig work and crunches it down in second. Yes I would spend 3 weeks making NC programs the old school way with trigonometry where the ball endmill would come in contact with a surface I was cutting. Slicing and cross sections I like regular surfaces. Once you got a pattern down then it was a easy to make a macro to surface machine those areas, but irregular surfaces had to be done step by step section by section then slice by slice.

Bottom line all things that seem equal are really not equal and where you may need to limit the toolpath in the areas and you will see different results. That is what I have done is draw a boundary around that areas and then scallop that area. Never said go figure it out as you have made a very difficult problem for the software to solve. It can do it, but you get what you get. You want exact results you take the time and draw the exact area you know if left make a boundary or just a surface trimmed of that area and you will get very nice motion in those areas.

Cusp Height Example

Picture was moved to give room on Emastercam click here.

Edited November 27, 2018 by 5th Axis CGI
Picture on dropbox to save room

[TERRYH]

Thanks Ron makes sense. Here is a picture of what I was working on the problem areas with the 1/4 ball was around the small ribs.

[crazy^millman]

I was thinking it was going to be crazy, but yes that would tax any CAM system in my opinion. The contact point of the 1/4 ball endmill is going to change greatly compared to the 1" and even the 1/2" ball endmill. That is what is doing the machining is the contact point of the endmill. Maybe someone from CNC can chime in, but since we are on the unofficial forum probably not going to get my of a response here. Either way you may find creating boundaries in certain areas or like I said take the time and trim areas of importance to just be those surfaces you want to machine and I would expect much different results. Free to solve it on it own solution then expect some weird results. Fun looking part and a 5 Axis Machine would machine that part very nicely. 

[Müřlıń®]

Legacy tool paths work in a bind and sometimes are the only way to fly.

But that type of work used to be my bread and butter.  one  reason you have a problem with leftover on the tool path could be that the tool radii and the finish corner on the model are the same.

most model software cannot put a perfect corner radii on parts like that so they will vary a couple thou one way or the other.  NURBS is an approximation and not an exact.

This wreaks havoc on leftover.  When I was modeling this type of work and only had the legacy paths to use, I would always make sure my corner radii I put on the model

was at least .005 smaller than my finishing tool I would be using to machine this.  Sometimes I would just leave the corner sharp.

The new high speed pencil will make a tool path that is almost identical to leftover except not do the hybrid constant z which iMO is not needed.

The new high speed paths work great for this type of work now and are not hindered by modeling quirkiness...

[Matthew Hajicek - Singularity]

I was just using Surface Finish Leftover on a vise jaw last night and had the same sort of thing.  Surfaces and solid faces that you think are tangent are really only very very close to tangent, since all software computes within a tolerance.  If there's any non-tangency at all, there's a chance your 1/4" cutter will fit .0000001" further in than your 1/2" cutter, which could jump a tolerance rounding from one .0001" increment to another, which means the software will think there's an uncut area that it needs to  handle.  It would be nice if we could tell it to skip areas below a specified size, but lacking that there are ways to improve it.  First try different tolerance settings.  Last night I tried the range from .001" to .0002", all with 20% filter, and found the best results at .0004".  There were still some undesired cuts, so I threw a containment boundary on it and got exactly what I wanted.

[TERRYH]

The radii in question were .270 so my thinking was the 1/2" ball should have finished them easily, and the 1/4" ball IMO should not have even tried to go back over them. However what Ron explained makes sense as to why it would look at them as still needing cut to an extent. And our 5-Axis machines are so backlogged right now they only want us to run thru them what is 100% necessary. thanks for all the replies.

[TERRYH]

Will using this help some in getting rid of what I seen on this part. Also I forgot to mention this is the 3rd or 4th one of these I have done all which had the same processes ran on them and this is the only one that had this issue with the 1/4" ball. 

[Müřlıń®]

.002... 50/50..... no smoothing on a part like that and I would use the high speed paths.

 

[ThomasJefferson]

On 3/16/2017 at 7:59 AM, TERRYH said:

We typically use the surface finish constant scallop to finish most not all of our parts, say we use a 1" ball then for the smaller corners we use say a 1/2" ball what tolerances do you guys use in this situation we typically use .0005 to .001 and I know the larger the tolerance the less it will actually do. I done this on a recent part and did the left over from 1" to 1/2" then a 1/4" balls, the 1/2 did a great job yet the 1/4" did some funky wavy cuts and jumped all over the place in areas it really should not have been looking at. Kind of confusing when we use the same process over and over and it does well one time and crap the next with the same settings.

That just seems to be the nature of Mastercam.   I run into this sort of thing all the time cutting mold detail.  There is no fix that takes care of everything.  I found that changing boundary to center and reset my upper and lower limits sometimes gets rid of some of the crazy jumping around.  Sometimes I need to add another in between tool (in your case maybe a 3/8 dia. before the 1/4).  Unfortunately this legacy toolpath still works way better that some of the newer rest toolpaths.  Another beef I have with leftover is the fact that MC does not seem to be aware of exactly how much stock is leftover and when a small tool goes into the leftover area, it gets buried in the stock and sometimes break.  (Can you say how much we need to drop parting line to fix that?)   You have to experiment a lot and hopefully find a work around.   WorkNC did a fantastic job with left over stock 20 years ago.  It's sad that Mastercam is still so far behind with this technique.

[AMCNitro]

Im not a huge fan of scallop, but many times its just the better solution.  I have found that if you leave .0005 of material it will smooth out the ragged tool motion that it comes up with.  I dont understand it, it works.  Try it

[Müřlıń®]

On 3/18/2017 at 10:29 AM, ThomasJefferson said:

  Unfortunately this legacy toolpath still works way better that some of the newer rest toolpaths.

WorkNC did a fantastic job with left over stock 20 years ago.  It's sad that Mastercam is still so far behind with this technique.

Perhaps you just don't know how to use them.

Leftover is a 20 year old solution and did a great job in it's day.

You are the one who is behind the times for not moving forward with the high speed tool paths, most of which are stock aware.

[ThomasJefferson]

10 hours ago, Müřlıń® said:

Perhaps you just don't know how to use them.

Leftover is a 20 year old solution and did a great job in it's day.

You are the one who is behind the times for not moving forward with the high speed tool paths, most of which are stock aware.

Thanks for reminding me why I hardly ever bother posting anything here anymore.

[Matthew Hajicek - Singularity]

Old, not obsolete.  There are several things the old toolpaths do better than the new ones.

[AMCNitro]

Hell, I still use 2d swept  A LOT.  I get way better finish on the molds we make than the other programmer that does almost everything with scallop...

[Matthew Hajicek - Singularity]

Yup, wireframe toolpaths, which are some of the oldest toolpaths in CAM, still produce the smoothest, most compact code.  (Compact code still matters.  I'm looking at Swiss machines and they come with 32 KILOBYTES standard memory, or about 280 KB expanded.  Yes, you can run off a flash card, but that introduces some limitations.)

Would you stop using 2D Contour just because it's old?

[crazy^millman]

Amazing I can flowline or HST a sphere and not get all arcs. I can 3D wireframe a Sphere and get all arcs. Filtering is not the same and has not been the same for a while now.

[huskermcdoogle]

I have been getting used to the old coons patch path.  I wish it had linking, roughing, translating and tool axis controls like in the moduleworks paths, would be stupid powerful for creating smooth no bs five axis paths for ball mills.

[Müřlıń®]

18 hours ago, ThomasJefferson said:

Thanks for reminding me why I hardly ever bother posting anything here anymore.

You have 6 posts....you appear to be a new user.   You come in here and elevate WorkNC above Mastercam and make incorrect statements about leftover and rest milling.

 Leftover is not stock aware...  it never was nor will be.

Sometimes legacy tool paths are the only way to go.  They are great tools to have in the tool box.

I built molds for 20 years using surface/finish contour/ surface rough pocket/....shallow.... leftover...pencil and flowline.

Those were my go to programs and I made them work extremely well and found all the nuances that made them act weird.

I would not go back to using those program's for all the tea in China.

The new high speed programs took just as much time to figure out as did the legacy programs if not more.

But once I figured it all out, they work extremely well.

Now I still have all the legacy icons on my quick access toolbar and like Ron and others pointed out,

there will always be a use for them in certain circumstances.

But for the most part the new High Speed paths blow them away and to say otherwise is incorrect.....IMO.

But that is just my opinion...

So don't take offence at my opinion...