What's new
What's new

Pros and Cons of TOOL EDGE vs TOOL CENTER

Who gives a shit what size cutter you'll be using?
Hand coding a simple profile is still, by far, a fuckton easier using full dia and part dimensions than trigging shit out for no friggin' reason!
Silly argument against full dia.
You don't like it? Fine!
You don't need it? Fine!
But claiming that your center line + wear comp is somehow superior is ...
Wow. Sounds like someone pissed in your Cheerios.

1. Perhaps your work is simple enough for that, but the vast majority of my parts do not consist of simple profiles.
2. No, I don't "trig shit out", I use CAM software. That's what it's for. It's far faster and much less error prone.
3. I care what size cutter I'm using, and not only that but what specific cutter I'm using, because I'm in business to turn a profit. When I'm programming, I know the part quantity, geometry, material, and what machine it will be run on, so I choose what I think will be the best cutter for the cut. The best diameter, flute length, reach, flute count, corner radius, coating, and brand. It's already chosen. Then I set what I think will be the best cutting parameters for THAT cutter in that cut. There is zero reason to use anything other than the cutter specified on the setup sheet, and any attempt to do so is a waste of time and money. If I caught an employee subbing out a different cutter without getting my approval first they'd get a stern talking to on the first offense, and probably see the door on the second.
4. Yes, little differences make big differences. One brand of .0295" carbide drill will fail after less than 50 holes in Ti6AL4V-ELI, while another will last over 12,000 holes (I'm still on the first one in one machine). One brand of two flute 1/4" uncoated will leave a beautiful finish on polycarbonate, while another looks like crap. Put in a 1/2", even of the right brand, and comp it out, and you'll melt the material because the SFM is twice as high as it should be. Put in a 1/8", and you'll get chatter and deflection due to the aspect ratio, and probably break it because the chipload is too high. Cutters are not interchangeable.
 
Wow. Sounds like someone pissed in your Cheerios.

1. Perhaps your work is simple enough for that, but the vast majority of my parts do not consist of simple profiles.
2. No, I don't "trig shit out", I use CAM software. That's what it's for. It's far faster and much less error prone.
3. I care what size cutter I'm using, and not only that but what specific cutter I'm using, because I'm in business to turn a profit. When I'm programming, I know the part quantity, geometry, material, and what machine it will be run on, so I choose what I think will be the best cutter for the cut. The best diameter, flute length, reach, flute count, corner radius, coating, and brand. It's already chosen. Then I set what I think will be the best cutting parameters for THAT cutter in that cut. There is zero reason to use anything other than the cutter specified on the setup sheet, and any attempt to do so is a waste of time and money. If I caught an employee subbing out a different cutter without getting my approval first they'd get a stern talking to on the first offense, and probably see the door on the second.
4. Yes, little differences make big differences. One brand of .0295" carbide drill will fail after less than 50 holes in Ti6AL4V-ELI, while another will last over 12,000 holes (I'm still on the first one in one machine). One brand of two flute 1/4" uncoated will leave a beautiful finish on polycarbonate, while another looks like crap. Put in a 1/2", even of the right brand, and comp it out, and you'll melt the material because the SFM is twice as high as it should be. Put in a 1/8", and you'll get chatter and deflection due to the aspect ratio, and probably break it because the chipload is too high. Cutters are not interchangeable.

Post copied for posterity
 
Gregor, I can offer one.
If you ever write some programs by hand, it is likely done with full dia comp.
If so, then you better make sure to enter the diameter into the offset BEFORE you run that program, and you better erase AFTER you ran it.
In my case, approx 10% of my mill programs, 100% of my lathe and 90% of EDM programs are hand-assist ( not hand trigged, but CAD drawn and hand coded ).
I also hand edit many ( most?) of my programs, where full dia just make much more sense.
As such, it would be an absolute nightmare to use two different methods.

Thankfully Featurecam creates full dia ( part line ) programs flawlessly even for roughing, so it is not yet an issue.
Might end up as an issue when I decide to move on from FC though.

That's certainly a valid reason for you - our workflows are very different, and this is not the first time we have had this kind of debate!

I am firmly in the zero hand coded programs camp. If something comes up that I really want to handcode for some reason, I do it as a manual code block inside my cam program. That way everything is posted out wholesale if I need to change something, and everything is self contained if I come back to it x years later. I tend not to do this often, as manual code blocks don't get simulated. Preferably I will use the toolpath editor to manually adjust a toolpath, which does get simulated. I use macros quite heavily, and often write custom functions to output code for them, no hand editing. API custom functions also do get simulated.

I also never hand edit posted gcode. If I don't like how something gets posted I fix my post, if I want it to be optional or variable in the post I make it optional or variable. If I want to manually optimise a toolpath I do so with the toolpath editor. All of my featurecam posts, even basic 2x lathes, are heavily customised with post variables so that I can make pretty much anything post exactly the way I want it to.

In short, there is no hand edit I could possibly do to the posted gcode that I can't make it post that way instead.

If the manual code block or edited toolpath are likely to be reused, add them to the part library so they can be quickly added to any new program.

OT, but I'm curious why, since you use featurecam, you don't use it's turning at all?
It's one of, if not the best turning cam on the market.

Again OT, but this setup is a large amount of work, and I can understand if some people find the payoff to not justify the time expenditure. At my previous job I was writing many programs every day, most of them for 1 off or low quantity fairly complex parts that would get run on one of a dozen machines by one of half a dozen operators, so I invested the time to do this. The data and workflow came with me when I moved on. This is what a lot of people do not get when I try to explain to them why switching cam systems is a fundamental and traumatic exercise.
 
OT, but I'm curious why, since you use featurecam, you don't use it's turning at all?
It's one of, if not the best turning cam on the market.
Mostly because I am wicked picky of my turning toolpaths, otherwise just a habit that I don't see the reason to change just yet.

Seriously, even the most difficult turned parts are done very fast with how I do them, don't see how to improve it.
 
If I'm doing simple turned parts, I just use the macros where possible, and do some hand programming. If I need to make curvier shafts, I use CAM. For milling, I always try to use CAM, except when doing 4th axis type parts that have a ton of radial holes; for those I write by hand with G83/G84 cycles. For all other milling work I try to use CAM wherever possible. I mostly do 3+2 type mill turn and 5 axis work. When I run VMCs I try to post directly from CAM, although I used to do hand programming years ago.

The best way to make complex parts is to go down to the local hardware store, buy the cheapest mini drill press you can find, chuck up a 1/4" jobber drill, and just slide your block of Inconel or Titanium around on the table with your left hand while you move the quill up and down with your right hand. I can hold tenths all day long with this method.
 
Mostly because I am wicked picky of my turning toolpaths, otherwise just a habit that I don't see the reason to change just yet.

Seriously, even the most difficult turned parts are done very fast with how I do them, don't see how to improve it.

That's fair enough.

I previously did a ton of long parts with very tricky internal features at horrible depths with non-existent clearances. I found that by far the biggest benefit of doing turning in cam was the simulation and being able to visualise tool clearances. So I just got into the habit of using cam for all turning I suppose. I'm very fast at it now, such that there is no time penalty over handcoding, and quicker in many cases.
 
But it will still run now don't it?
At the same time, the program won't run with a larger tool and scrap it now does it?

That said, me thinks you're just trying to make an argument for your style of programming.
How many here optimizes the very last bleeding 1% out of their programs?
Not that I use many regrinds for finishing ( they are typically relegated for roughing with comp ), but often I switch to a metric EM for finishing in tight corners, all that without having to repost or change anything in the program.
roughing with comp? surely not adaptive style roughing paths right? i've not seen 1 cam that will put out wear comp in a roughing path, not that you couldnt do it manually...
 
Most of our lathe programs are very simple so I hand code them and use TNR. Simple mill stuff I hand code and use full diameter. 5 axis I use CAD and wear . Some of my 5 axis work is so close to the fixture I will not take a chance of changing tool size or holder type.
 
that tells me nothing, what kinda toolpath is it?
I'm not sure what you're asking?
You've said you've never seen CAM output comp for a roughing path.
I showed you that Featurecam does in fact do that.
Regardless of the toolpath, comp is only applied for the final pass when the tool is on the contour.
 
I'm not sure what you're asking?
You've said you've never seen CAM output comp for a roughing path.
I showed you that Featurecam does in fact do that.
Regardless of the toolpath, comp is only applied for the final pass when the tool is on the contour.
i'm guessing its not an 'adaptive' style toolpath. thats what i'm referring to. traditional style 'pocket clearing' paths i know you could apply wear comp.
 
i'm guessing its not an 'adaptive' style toolpath. thats what i'm referring to. traditional style 'pocket clearing' paths i know you could apply wear comp.
OK, so I will clarify this one more time: The comp is applied ONLY on the final roughing path when the tool is clearing up the contour.
In case of a pocket or a boss or whatever, the tool goes about it's business to remove material where needed, and then makes a final path along the profile as to leave a constant amount for the finishing tool.
It is there and ONLY there where the comp is applied.
All other places comp is Off.
 
OK, so I will clarify this one more time: The comp is applied ONLY on the final roughing path when the tool is clearing up the contour.
In case of a pocket or a boss or whatever, the tool goes about it's business to remove material where needed, and then makes a final path along the profile as to leave a constant amount for the finishing tool.
It is there and ONLY there where the comp is applied.
All other places comp is Off.
i get that. sounds like an old school pocket clearing toolpath, not adaptive.
 
OK, so I will clarify this one more time: The comp is applied ONLY on the final roughing path when the tool is clearing up the contour.
In case of a pocket or a boss or whatever, the tool goes about it's business to remove material where needed, and then makes a final path along the profile as to leave a constant amount for the finishing tool.
It is there and ONLY there where the comp is applied.
All other places comp is Off.
Which requires that the correct diameter cutter is in the machine for the roughing passes.
 








 
Back
Top