| | |
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.
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.
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.
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.Originally Posted by mattpatt
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.
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!
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
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.
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
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.
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.
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 :-)
Posting Permissions
| | |
LinkBack URL
About LinkBacks
