[mattpatt]

It appears from looking through the tutorials that roughing requires a work area profile, whereas finishing works best with selected faces. Can anyone confirm this?

I had a profile and the finishing seemed to go ok, until I used the angle limits on constant z finishing. At this point everything locked up and it wasn't happy. Changed to selected faces and it worked as intended.

[Brakeman Bob]

You can use both at the same time if you wish. I used to use Work Area all the time in 3D finishing - now I have HSM I find the Silhouette option more useful.

I tend to use Faces when I need to leave particular faces unmachined or with a finishing allowance on.

[mattpatt]

Thanks for the reply Brakeman Bob.

Up until today I wasn't having trouble. T'was only that it didn't like the angle limit thingy that I decided to look into it a little further.

How do you find the HSM option compared to 3D machining? I'm still a novice so I don't think I'll get myself into that yet, but it's worth noting for the future. Does it save a lot of time? Tool wear etc? At least, that's what it claims in the brochure!

I'm on a steep learning curve here, but I don't want to get out of my depth just for the sake of it.

Matt.

[Brakeman Bob]

How do you find the HSM option compared to 3D machining? I'm still a novice so I don't think I'll get myself into that yet, but it's worth noting for the future. Does it save a lot of time? Tool wear etc?

I find it very good, especially doing very curvy faces. You have much more control of what the tool does on its lead in and lead out, the are some very nice cutting strategies (I especially like the combined Z Level and Linear with a control to say at what angle one strategy changes to the other) and the boundary constraints have more options. It does save time, but I haven't done the sums to say how much - I implemented a lot of things at same time we took up HSM such as 5 axis, gundrilling, plunge roughing to name but three and to single out the gains from one particular innovation would be a lot of hard work. One thing I would say is it does help make older machines cut quicker as the decleration and acceleration when the tool changes direction is in the code rather than relying on the acc & dec in the servo parameters to sort it out.

If you are doing Mould & Die work I would say you really need to look at HSM because it to my mind it seems developed with that industry in mind.

[mattpatt]

Thanks for the reply Bob.

At the moment I'm only doing runs of parts, not moulds or dies. However, I've recently been talking to a company from France who need some parts made. They asked for a couple of sample parts, which I made, and they were happy, and they've just giving me a few more drawings and on a few of the parts there's a large amount of roughing involved, so any time saving here would make us all winners.

How accurate is the time taken during the simulation? Would it at least give me an idea if it's faster or not?

As for 5 axis etc. My FADAL/FANUC is just 3 axis at the moment, with a possible future upgrade to 4 axis, but 5 axis certainly presses my buttons :-) Then again, it's taking all my time getting proficient in 3 axis so I'll have to cancel sleep time if we add another axis!

[Brakeman Bob]

How accurate is the time taken during the simulation? Would it at least give me an idea if it's faster or not?

I wouldn't trust the time shown in SolidVerify. I know from what I do that it grossly exaggerates the dime to drill holes and under-estimates the time to machine 3D. The latter is normal for all CAM systems, though I am not sure about VeriCut or NCSimul as these may have values in them for the acc / dec of the machine. I used to work in Applications for a machine tool builder and for reasonablely accurate time studies I used to do it the old fashioned way with distance in cut and feed per minute. When the thorny issue of 3D machining came up I used a blanket allowance for acc / dec (between 20%and 35% depending on the machine) which I had arrived at empirically with shopfloor trials. Some CNC editors show the distance travelled by a cutter in G1 and G0, so it is a simple sum to calculate the time in cut then compare this to the actual time taken to machine that code. Do that a few times with different jobs (but with the same tool) and you will soon get an idea of what your machine is losing in servo response. Bear in mind that bigger moes have smaller losses than smaller moves, so the surface tolerance set in SolidCAM will have a big impact on the cycle time.

All the best

Bob

[mattpatt]

Having a play with HSM. I've got a job with some pockets that I want to machine, and I'd like to pre-drill the entry. I've done this already using 3D drilling prior to 3D milling and it works fine, but I can't find this option available in HSM. When the tool moves to the pocket area it doesn't see the holes (in HSM) and enters the job in a helical move. Not a huge problem but I'd like to use the drilled holes as the entry if possible.

I see in the Contour roughing/link/strategy page that there's a section marked "pre-drilled entry points". What is this as I can't find any info?

Hopefully someone can help me here.

Thanks.

Matt.

[Brakeman Bob]

Hi Matt,

You are ahead of me on this one - I almost never use the pre-drill in pocketing and almost never use HSM for roughing. If I have big enclosed pockets to deal with I use a ramping strategy in 3D milling or a plunge mill strategy with a U-Drill cutting half-holes (Sandvik's series 880 are good at this).

Bob

[mattpatt]

Interesting.

Well, I haven't actually mounted the job on the machine yet, as I'm still trying to come up with the best method of machining, and the clumsy oafs at the anodizing factory decided to throw all my last batch of parts in one box with no packing material, so they're all dinged and scratched and need a bit of remachining to save them, which has put me off schedule a tad.

Anyhow, I'd like to give the HSM Contour roughing a bash, just for a look, and then a selection of other 2.5D and HSM rest and finishing ops to get the job done.

I really like the way the toolpath 'leaps around' in the simulation, but it's difficult to follow, and I'm looking forward to see how this goes during real time cutting.

[jmcglynn]

Hi Matt,

You are ahead of me on this one - I almost never use the pre-drill in pocketing and almost never use HSM for roughing. If I have big enclosed pockets to deal with I use a ramping strategy in 3D milling or a plunge mill strategy with a U-Drill cutting half-holes (Sandvik's series 880 are good at this).

Bob

Bob, why not HSM for roughing? I tend to use it a lot for roughing, and use non-HSM for finishing in some specific cases. For 2D shapes and pockets HSM is a bad choice for finishing because the surface finish if terrible (loads of little fidgety little arc moves).

Joe

[Brakeman Bob]

Bob, why not HSM for roughing? I tend to use it a lot for roughing, and use non-HSM for finishing in some specific cases. For 2D shapes and pockets HSM is a bad choice for finishing because the surface finish if terrible (loads of little fidgety little arc moves).

Joe

Joe, I don't use HSM for roughing because I block the part out using 2D profiles and pockets. I do use 3D roughing for small pockets because I use plunge-milling for roughing 3D shapes and I must admit I don't know if that strategy is available in HSM - I haven't looked.

[mattpatt]

Just did a job and it was my first attempt at rough contour cutting with HSM.

Now, I'm not really high speed machining, but I wanted a play. When I timed the operation during real time cutting the difference between simple pocket milling and HSM wasn't a great deal (HSM was quicker), but the difference was that I was able to control the cutter engagement much better, and if you ask me this means less chance of the cutter breaking, and less cutter wear.

It was also really smooth coming out of the part and re-entering, which is where I think the time saver was.

Now all I need is more rpm and I can get this thing really ripping :-)

[Brakeman Bob]

Hi Matt. I am glad you liked HSM. I find that on jobs with a lot of 3D (I'm talking 10 million lines of code upwards) HSM gives a real time time saving. You are right in that the lead in/out and the links are smoother and this is where the time is saved as the machine isn't straining the acc & dec so much and therefore getting closer to programmed feed.

Another plus with HSM is you will get better 3D finishes that display less facetting than the vanilla 3D routines. The combined strategies are very useful too, as are the options for constraining the tool working area. However, it ain't honey and roses all the way as I find the roughing strategies in vanilla 3D more useful, especially the plunge and trochoidal milling. Still, it is stuff like this that makes CAM such an interesting thing to do for a living isn't it?

Have fun.

Bob

[mattpatt]

CAM is most interesting indeed, but can also be very frustrating when it doesn't generate like you'd want it to.

It's a shame that it's only a part of my job, as I'd like to spend more time on it, but I just don't get the chance.

However, when I see the finished job it's great to know that I made it, start to finish. From idea to finished product. I used to do my own anodizing as well, but my neighbours complained about the smell of the acid, so finally had to farm that out!

[Eclipze]

I've done quite a fair bit of 3D milling, but the one area I struggle with is increasing the speed of movement. I would really prefer to be running at 1000mm/min or above, however for 3D surfaces it slows right down to ~250mm/min. I can reduce the step size with the facet tolerance (large gcode file) and increase the acceleration, however it get to a point where the CNC is shuddering under the rapid accel/deceleration from point to point movement. The shuddering causes additional tooling marks in the surface of the work piece. So I have to reduce the speed.

It appears that Solidcam only generates the profiles with small linear steps, and the resulting movement is stepwise/jerky. Does anyone know if there are any techniques to produce gcode that provides a smoother/faster movement? Does HSM improve on this limitation?

[Brakeman Bob]

I've done quite a fair bit of 3D milling, but the one area I struggle with is increasing the speed of movement. I would really prefer to be running at 1000mm/min or above, however for 3D surfaces it slows right down to ~250mm/min. I can reduce the step size with the facet tolerance (large gcode file) and increase the acceleration, however it get to a point where the CNC is shuddering under the rapid accel/deceleration from point to point movement. The shuddering causes additional tooling marks in the surface of the work piece. So I have to reduce the speed.

HSM would help here and without being more familiar with your machine it is hard to say how much. An awful lot will be down to the machine, the servos and the control. For example, how many blocks ahead is the control reading? Is your control "smart" such as FANUC HPCC? How are powerful are your servo's and are they tuned correctly? When you say you increase the acceleration, do mean you put the gains up and/or the acc & dec? This could be the cause of the trouble as without proper tuning with an oscilloscope, high feed rates can give rise to axis instability.

Have you got access to a ball-bar? If so, run ball bar tests at 500, 1,000, 2,000 and 5,000 mm/min. This will give you a very good idea to the capabilities of the machine. When I worked for a machine tool builder our standard ball bar test was 3,000 mm/min at 150mm radius.
The shuddering you describe at those low feed rates could indicate all is not well with your ballscrews and a ball bar test would show that up straight away.
To give you an indication of what I expect from the machines in our shop, we have a Mori Seiki SH400, 10 years old with Fanuc 16MA and for 3D milling Aluminium I program a Ø6 ballnose at 12,000 rpm and 3,000 mm/min. On very curvy geometry prior to HSM, the machine made it up to about 2,000 mm/min. Programming with HSM and the machine managed to get up to about 2,600 mm/min. And the machine wasn't shuddering, the lost feedrate was due to the movements being too short for the machine to get up to it's full velocity.

[Eclipze]

Thanks for your reply :-)

The CNC runs 305oz/in stepper with Gecko G203V drivers and Mach3. I use the DIN_ISO CNC controller in SolidCAM. The acceleration parameters are set it Mach3. I can easily traverse 3500mm/min without stepper dampers, however usually only cut around 1,000mm/min.

Not familiar with ball bar tests, however looking into it I believe the root cause is the way the gcode is generated. For example, if I do a 2D profile with curves, the end mill will slice through the material and not slow down around the corners. The gcode uses commands to perform arcs. Whereas in 3D milling, the entire gcode is point to point. Any profile curves are now made up of small straight lines between two coordinates.

The limitation of the CNC is the maximum acceleration before the machine flexes (only a small machine). So if I stop with a deceleration of 500, it stops perfectly, but the momentum energy dissipates as a little bit of machine flex from the sudden stop. When this happens running the 3D milling code, it produces a shuddering noise around tight corners, though will reach maximum feedrate where straight sections are machined. The shuddering causes slightly more machining marks on the surface of the material.

So a 2D circle utilising gcode commands for arcs is very smooth and very fast >1000mm/min. A 3D milling operation however falls below 350mm/min and shudders it's way around, where only point to point gcode is utilised.

At this stage, I am unsure as to whether a solution involves optimising settings, or whether it's a limitation of Solidcam or one of Mach3.

[Brakeman Bob]

The limitation of the CNC is the maximum acceleration before the machine flexes (only a small machine). So if I stop with a deceleration of 500, it stops perfectly, but the momentum energy dissipates as a little bit of machine flex from the sudden stop. When this happens running the 3D milling code, it produces a shuddering noise around tight corners, though will reach maximum feedrate where straight sections are machined. The shuddering causes slightly more machining marks on the surface of the material.

I think HSM will help a little, but not much as this is a machine dynamics problem and HSM's only contribution would be to smooth out the sharp corners. The only software that I know of and that would be of benefit is OptiPath from VeriCut. This looks at a tool path and then applies a feedrate for every block, effectively hard coding the acc & dec into the machining program. very expensive, especially as you have to buy a seat of VeriCut to enable OptiPath to run.

Is the acc & dec in Mach3 straight line or ramped? If ramping is available, try changing the ramping co-efficient. Or perhaps there is a parameter for changing acc & dec depending on the distsnce to be travelled in the block.

On the ballbar thing, I used to run tests with the ballbar path programmed as G01 interpolation to test acc& dec response.

[Eclipze]

Mach3 has linear trapezodial ramping profiles for each axis, and does not have any other related adjustment. I've played around with different accerations, however there is a point where it slows down the feedrate through corners. When too high, the jerky stepping becomes more pronounced.

Perhaps the problem is related to how the gcode is interpreted. I'm not sure if every CAM software generates the same point to point steps for 3D milling (where no advanced gcode commands are available to improve the trajectory), or whether it is a limitation of the Mach3 software in how it interprets the gcode. Whereby it accelerates to a point, decelerates approaching the same point, then accelerates away from the point. If is were to look ahead and plan the transistion from one point to another, could it be smoother? I guess this statement is suggesting any such "smoothed" transistion between two points implies requires some sort of non-linear curve, which may not be exactly expected. But with a fine enough resolution, it wouldn't necessarily be an issue.

Thanks Brakeman Bob... you've got me thinking in a few directions that might solve this one. Perhaps with the next small 3D milling job, you could help with generating a 3D milling operation so I compare the HSM with Solidcam to see if there is a difference.

[Eclipze]

Problem SOLVED!!!

First I'd like to specifically point out the issue was not with SolidCAM which I had previously questioned. The jerky motion was if fact to do with Mach3.

Mach3 has two motion control modes, Constant Velocity and Exact Stop. This is set under the Config --> General Config. I did have it on constant velocity, but it was acting like exact stop mode. In the Setting tab (Alt-6), there is an option for "CV Feedrate", which was enabled. I turned this off and the difference it quite apparent. I could turn it on and off while air cutting and it's a BIG difference. With it off... very smooth and the indicated feedrate remains at the 1000mm/min. Turn it on and during 3D corners it would erratically slow right down to below 300mm/min.

I would recommend other Mach3 owners consider trying this, as it should improve the cut finish and reduce fatigue/wear on the CNC.