[pete from TN]

I have been using this machine I built now for a little while. It is working well and I have purchased Sheetcam to use as my cam program for 2.5D projects. It is a great program and has made it possible for me to do some really cool stuff. I am using Mach3 which is also very nice altho I have been considering having a look at EMC. Currently I am using the Sheetcam tooltable I made to track all of my tools and their individual offsets. I am using the TTS tormach style toolholders and I really like that they can maintain great Zero repeatability. So far all of my programs have been using the tooltable in Sheetcam and I have never done one in Mach3 on the machine. Before that I was just doing my drawings and zeroing every tool on the work until I figured out how to use the tool length offsets. My question then is I am wondering how many of you do your machining setups this way? Do most of you use the cam programs offsets or mach3 and how do you let the cam program know what to do if you use mach3's table? IS there a particular way that they work together? I have been doing well with this but my concerns lie in the fact that I am trying to get into 3d machining techniques and that is beyond the realm of sheetcam so all of my tool length offsets are gonna then be obsolete. Would you say that it is more useful to just use the mach tooltables and import a cam profile that just calls up a tool? I have been curious about this for a little while now and I just thought I would ask all of you guys what you do on your machine?

Also what are you 3D guys using for Cam that is not ridiculously expensive? That is my next adventure.... peace


Pete

[ihavenofish]

I have been using this machine I built now for a little while. It is working well and I have purchased Sheetcam to use as my cam program for 2.5D projects. It is a great program and has made it possible for me to do some really cool stuff. I am using Mach3 which is also very nice altho I have been considering having a look at EMC. Currently I am using the Sheetcam tooltable I made to track all of my tools and their individual offsets. I am using the TTS tormach style toolholders and I really like that they can maintain great Zero repeatability. So far all of my programs have been using the tooltable in Sheetcam and I have never done one in Mach3 on the machine. Before that I was just doing my drawings and zeroing every tool on the work until I figured out how to use the tool length offsets. My question then is I am wondering how many of you do your machining setups this way? Do most of you use the cam programs offsets or mach3 and how do you let the cam program know what to do if you use mach3's table? IS there a particular way that they work together? I have been doing well with this but my concerns lie in the fact that I am trying to get into 3d machining techniques and that is beyond the realm of sheetcam so all of my tool length offsets are gonna then be obsolete. Would you say that it is more useful to just use the mach tooltables and import a cam profile that just calls up a tool? I have been curious about this for a little while now and I just thought I would ask all of you guys what you do on your machine?

Also what are you 3D guys using for Cam that is not ridiculously expensive? That is my next adventure.... peace


Pete

ive never used tool tables and offsets. ive done everything manually tool by tool (even though i do have a few tts tools). ill be getting around to changing that pattern soon.

ive been using a couple different things to make my 3d cutting programs, but its really hard to get around the price point.

for modelling, i use 3d studio max primarily. im a computer animator, so i know how to use it, and more importantly its been paid for. the reasoning behind this odd choice is that there is a free set of gcode and toolpath generating tools for it. very basic, but quite usable if you know 3dsmax well and in my opinion, nothing beats polygonal modelling for freeform shapes (they do slow down the cam though).

the other thing ive just gotton is visual mill. it came with my new machine. i think retail is $1000. so far i think i like it. its been pretty easy to get the hang of it, and seems to cover the most important functions. ive just finished my first complicated part with it and hope to machine it tonight. its a small guitar bridge. theres 11 operations, 3 tools, and it took me maybe 2 hours to set up, if that. this part is more of a 2.5d part, but the 3d tools are just as easy to deal with (ive done a contoured guitar body but havent cut it).

the hard part for me has been figuring out what to model, and what not. when i make something for a design, i model everything including chamfers, fillets draft tapers and all. for cam though, you want to deliberately leave those types of features out, because you need the "true" edge to reference for chamfers and the like.

[pete from TN]

That sounds like it should work alright. I have been playing with Alibre for 3d cad and I have not decided on my cam yet. I think I understand what you are saying about the leaving out the champfers. I do that with sheetcam too and just use work offsets to arrive at the desired champfer. I have been using tool offsets now for awhile and I gotta say it is the way to go over zeroing every damn tool... that gets old real quick. However I was wondering about others use of the tooltable and if they mostly rely on mach to hold the offsets and then use the cam program to call up the operations with no offset. I assume it would work that way altho I do not know. I just had a crappy incident happen where I had some kinda computer fluke and lost all my tool length offsets in sheetcam. I was kinda okay with it because I wanted to make my zero tool or number one tool the shortest so all the rest are positive offsets which I did not have before. I cut and turned my zero tool shank on the mill today and redid all my tool offsets. Kinda a PIA but glad it is working again. I just got thru machining a fixture for another project I am working on with them and so far so good. The 3d cam vectrics stuff looks good too tho... I like that they have a lot of free profiles and you can buy some others for reasonable pricing.... peace

Pete

[gd.marsh]

Not far enough along with my mill to get into the tool table issues ..

I can comment on Vectric Cut3D though .. We use both Cut2D & Cut3D with the CNC Router (re-zeroing every tool) .. I do intend to continue using them once my Mill Conversion is complete also (with a tool table set up)

So far we have not found a situation where Cut2D & Cut3D couldn't accomplish what we needed. On occasions there are minor g-code tweaks to make sure there's ample rapid tool height in certain areas or little things of that nature, but the g-code is solid.

2 sided parts are a snap once you figure-out how to register the material correctly on both sides. We've had good results with that. Haven't run into a need for slicing yet, but I recall reading about some drawing modifications that need to be made when slicing a part that's being cut with a ball end mill.

But IMHO - The price is right and the software is good!

[cyclestart]

Tool length offsets in the control, Mach in this case.
Cam creates code that calls for tool length offset from control. Example "G43 H01" for tool #1.

Isn't that the normal way ? Something tells me I'm misunderstanding the question.

[pete from TN]

Vectric software is high on my list of possibilities.... here's my question for you.... What do you NOT like about it? What can't it do? I am getting a little more proficient with my 2dcad and have been experimenting with Alibre I have here and starting to " Get it" so I am hoping to be there soon. One of the things I really want to be able to do is machine a Lithopane on my mill. If I have to rig up a HSS I will do that but I think I can do it with the 6K I have now and if I want to bump it up a tad I can do that as well....

The tool tables are a VERY important part of this stuff if you ask me. Now that I am using them I cannot imagine not using them.... Doing all my programming in Sheetcam and just snatch a toolholder and stick it in the machine once you have that initial Zero is just too much easier. Unless of course you are like my Pal Art who has the whizzbang custom tool height offset sensor setup on the table and never has to zero a tool again.... Damn that guy is clever!!!

I am just not getting the Mach3 tool table setup in association with the cam work. Sheetcam virtually begs you to have a tool table. You do not need to use offsets if you do not wish to but you must choose a tool and give it parameters so the program can figure the cut path... I suppose in Mach with a tooltable you would just set everything for zero offset and call up the tools in your mach tool table but I am not sure how Mach will figure the offset or not.... HMMMMMM


Peace

[gd.marsh]

Mach tool table ..

I may be way out in left field on this .. but wouldn't you want your tool table in Mach so the program can tell you which tool to run next & also accurately report the tool's diameter? Seems to me that info showing up right on the screen would make for less chance of grabbing the wrong tool and ruining a part.

Gary

[pete from TN]

Well currently the way I am using Sheetcam the tool operations are done one by one and when the toolchange needs to happen mach will raise the millhead to a toolchange position I designate, alert me that the next tool is tool whatever, and wait patiently for me to fumble around putting the next tool into the spindle and tightening the drawbar and then I hit cycle start again and the program continues.. It really is pretty slick this way but I gotta imagine that Mach3 has other ideas about toolchanges that might perhaps be even better. Ya see when I do a part in sheetcam I have to select the cutting operation and the tool to use for it. In times like todays drama where I lost my tooltable information and had to redo all the tool table settings which are now different all of my saved sheetcam jobs that were proven and worked fine are now wrong.... That is until I reopen each file and load the NEW default tool table and the program automatically updates itself. I usually just go in there and recheck everything to make sure. What I do not know is how Mach3 would do this assuming I only set all of my tool settings in my cam program for a work surface zero reference.... That was why I asked about this to see if there is anyone who is actually using their machines and might be doing things differently/ better than I am.... peace

Pete

[SCzEngrgGroup]

The tool table HAS to be in Mach3 to work correctly. SheetCAM does not actually apply tool offsets, it simply inserts the appropriate G43 and G49 commands to apply and remove the appropriate offset for the current tool.

In general, tool offsets in the tool table are setup at the beginning of each job, using a touch-off plate, or by measuring each tool separately, and storing the numbers away somewhere. Unless you have tool holders that give a precisely consistent Z position, using the tool table is a waste of time. Tormach holders, and R8 endmill holders are the cheapest and easiest way of getting this. Forget about using collets, drill chucks, etc., unless you come up with a means of controlling how far into the collet the tool goes when you install it. Using offsets also doesn't really save any time or bother unless you either work with a small number of tools on all your projects, so you can just leave a single table loaded all the time, or you're doing "production" runs of identical parts. Just doing one part, witha unique table, it won't save you any time over doing manual changes and just touching off each tool as you install it, unless you have to use each tool several times for that one job.

Regards,
Ray L.

[pete from TN]

But sheetcam DOES apply the offsets and everything I have machined since I made my sheetcam tool table has worked that way. I DO NOT have a mach 3 tool table at all. That is why you install the tool offsets into the tables in sheetcam so that you can use them. I do use TTS tooling that has a repetitive Z reference and I have installed all of the tools I have into it. I basically have around twenty toolholders that are being used. Some collet holders, some setscrew holders, and a few drill chucks. This ABSOLUTELY speeds up production because all of the products I have been making are made with some variety of all the previously setup toolholders I am using. I just zero on the part surface with my number one tool which is a solid rod, then start the program, it requests the first tool, I install it, and then the machine does the rest until the next tool change. The only way mach has these tools installed is if by some sheetcam wizardry it magically installed them. I know I did not.... However what I am asking here is not wether or not what I am doing will work, It certainly does, rather if I use Mach3's tooltable would that somehow be better and how? does that make sense? peace

Pete

[pete from TN]

Think of it like a commercial VMC ( I WISH) in a commercial VMC you might have a 20 or 25 tool carousel. If your shop is worth its salt you will have the thing stuffed with all of the most commonly used tools and cutters that will make the majority of your jobs. These tools are programmed into the machine and their offsets loaded so that the machine can call up any tool and be on the zero automatically. Then your cam setup will just call a particular tool and you setup your zero for whatever part of the material you need to and youre hopefully done. That is what I am basically doing and that is what I am after hopefully with any future cam programs that may or may not have that capability. WHich is why I am wondering if the tool table in mach is the best place to setup these offsets? peace

[ihavenofish]

im gonna have to try these offsets just to see how they work. you can enter them in mach, and you can enter them in cam by the look.

in theory, i dont imagine it matters, as long as the one you use is correct. in a big work environment with many engineers and machine operators, i imagine setting them in the machine is the only realistic way to keep things managed, as the offset of the same tool might be different in every machine.

fun fun. i did run my part tonight, and it worked rather nicely. the chamfer was wrong however due to user error. i mistakenly thought my spotting tool was a sharp point. its actually got a small land on it. easy fix. visual mill has a special chamfer operation. you just select the edges, amount of chamfer, and "overbite" (amount the tool extends past the chamfer).

[mwood3]

I think an easier way of explaing the tool table in mach would be like this.

as far as your cam program goes it will try to put the face of your spindle to the depth of your cut when the G code is run...this is where the Mach tool table takes over...you tell mach the length of each tool and it will compensate for it automaticly.

your current system works but I can see it being a PITA when you wear out or break a tool...even with TTS tooling no 2 tools will be ground the same length. this is where the mach tool table shines, just make a jig to hold the tool holder and a height gage to measure the distance from the surface that seats against the spindle to the tool tip...

If that didnt make sense imagine an upside down spindle with a surface you can zero your height gage out on(nose of the spindle) then measure to the tip of the tool...

edit: one more thing, when you call a tool you will have to put in tool comp codes ie: G43 H1 = apply tool offest for tool 1

[pete from TN]

So what you are saying is that Mach would normally call up the tool offset as directed by the cam engine and automatically account for it in the machine control. I do not however see your point as my way being a pain in the keister as it really does not matter if your tool breaks or is replaced because you still have to measure the tool length in any case and wether you input it at the machine or in the Cad room in the house it really makes little difference no? For instance I just had to redo all of my tool table as it was lost somehow in my computer, and I changed my tool number one or my reference tool to be the shortest one and I was able to remeasure all of my tools in just about a half hour.... So the only reason I can see right now for me to change the tool table to mach or at least to copy it to mach would be for software I may buy in the future that does not have this capability. I cannot imagine a cam system tho that does not have tool information in it since that is the meat and potatoes of the thing right.....

Dunno how my machine has been working all along without a mach tool table but I have not installed anything tool related into mach and it still works fine. You can load your tool information into sheetcam sans the offsets which if you do not enter anything there it is Zero and then you can either zero every tool on the surface or setup your tool table in mach I suppose.... Is there any other advantage to using it in mach that has not been discussed? peace

Pete

[ihavenofish]

So what you are saying is that Mach would normally call up the tool offset as directed by the cam engine and automatically account for it in the machine control. I do not however see your point as my way being a pain in the keister as it really does not matter if your tool breaks or is replaced because you still have to measure the tool length in any case and wether you input it at the machine or in the Cad room in the house it really makes little difference no? For instance I just had to redo all of my tool table as it was lost somehow in my computer, and I changed my tool number one or my reference tool to be the shortest one and I was able to remeasure all of my tools in just about a half hour.... So the only reason I can see right now for me to change the tool table to mach or at least to copy it to mach would be for software I may buy in the future that does not have this capability. I cannot imagine a cam system tho that does not have tool information in it since that is the meat and potatoes of the thing right.....

Dunno how my machine has been working all along without a mach tool table but I have not installed anything tool related into mach and it still works fine. You can load your tool information into sheetcam sans the offsets which if you do not enter anything there it is Zero and then you can either zero every tool on the surface or setup your tool table in mach I suppose.... Is there any other advantage to using it in mach that has not been discussed? peace

Pete

the things hes talking about with tool breakage is that if youve made a program you need to run 100 times, and break a tool, its easier to measure and enter into mach than to measure and got back to cam and re-export the gcode.

unless im missing something (i suppose you can simply write it int the gcode file manually).

[pete from TN]

I can see having to redo the code might be a pain but I have broken bits before and basically all I did was replace it with a new bit and set the new bit for the same offset as the old one. This time I have a list on paper I keep by the machine in case the computer farts again. Before that I would just go to sheetcam, open the saved job, open the tooltable and look at the offset. Take it outside and setup the new tool to be that same offset. Not really much difference and this way you need not redo the code.... I usually just set my tool number one in the machine, zero it on a surface, then replace it with the new toolholder and input the offset into MDI and then bring the tool down to that same surface by hand and tighten the collet nut or setscrew.... pretty easy really...

I am not looking for reasons NOT to change what I am doing here rather I am looking for a GOOD reason to change what I am doing and so far the only thing that really jumps out at me is FUTURE cam programs and how they might interact with mach. Does anyone here use thier tooltables? Perhaps I should have asked this question over on the tormach forum since they are all probably using thier TTS holders this way perhaps? Peace

Pete

[SCzEngrgGroup]

But sheetcam DOES apply the offsets and everything I have machined since I made my sheetcam tool table has worked that way. I DO NOT have a mach 3 tool table at all. That is why you install the tool offsets into the tables in sheetcam so that you can use them. I do use TTS tooling that has a repetitive Z reference and I have installed all of the tools I have into it. I basically have around twenty toolholders that are being used. Some collet holders, some setscrew holders, and a few drill chucks. This ABSOLUTELY speeds up production because all of the products I have been making are made with some variety of all the previously setup toolholders I am using. I just zero on the part surface with my number one tool which is a solid rod, then start the program, it requests the first tool, I install it, and then the machine does the rest until the next tool change. The only way mach has these tools installed is if by some sheetcam wizardry it magically installed them. I know I did not.... However what I am asking here is not wether or not what I am doing will work, It certainly does, rather if I use Mach3's tooltable would that somehow be better and how? does that make sense? peace

Pete

Pete,

So you're not using G43/G49 then? SheetCAM is just fudging the Z position depending on the tool you use. Interesting.... I can see how you can get away with that on a single Z axis machine like your 45. My knee mill makes it more complicated, since I have limited "Z" travel on the quill, and have to apply the tool length compensation using the knee. I had to write custom Mach macros to do that correctly, and have to use them in place of G43/G49.

So how do you handle non-repeatable tools like drills? On mine, before starting a program, I touch off all the tools used by that program, which loads the tool table automatically. I have custom macros to do this, so it just takes a few minutes. But you have to put the offsets into SheetCAM, then re-generate the G code, right?

If you have less than 253 total tools, putting the offsets into Mach would allow you to zero all the offsets in SheetCAM, and have offset-agnostic G-code, with the offsets applied by Mach3 when you run the program. Right now, if you change any tool, even if you just re-grind a drill bit, you have to regenerate all your G-code. Kind of a pain if you break a drill in the middle of a job, or run your endmill into a clamp (not that any of us would EVER be dumb enough to do that, right?) and have to swap it out. With the table in Mach3, you'd just update that one entry in the table, and then continue the program from where you stopped it when the tool broke, using the exact same G-code.

Not a big difference in most cases, but a difference.

Regards,
Ray L.

[SCzEngrgGroup]

I can see having to redo the code might be a pain but I have broken bits before and basically all I did was replace it with a new bit and set the new bit for the same offset as the old one. This time I have a list on paper I keep by the machine in case the computer farts again. Before that I would just go to sheetcam, open the saved job, open the tooltable and look at the offset. Take it outside and setup the new tool to be that same offset. Not really much difference and this way you need not redo the code.... I usually just set my tool number one in the machine, zero it on a surface, then replace it with the new toolholder and input the offset into MDI and then bring the tool down to that same surface by hand and tighten the collet nut or setscrew.... pretty easy really...

I am not looking for reasons NOT to change what I am doing here rather I am looking for a GOOD reason to change what I am doing and so far the only thing that really jumps out at me is FUTURE cam programs and how they might interact with mach. Does anyone here use thier tooltables? Perhaps I should have asked this question over on the tormach forum since they are all probably using thier TTS holders this way perhaps? Peace

Pete

Pete,

Look at it this way: Your system works fine, but every time you want to run a program, you probably need to generate new G-code, in case any of your tools were changed out since the last time you generated the G-code. If you don't, and a tool has changed, then your part will come out wrong. If you use the Mach tool table, the G-code doesn't care what the tool lengths are, as the machine will apply them when you run the code. When you change a tool, you re-set the offset for that tool in Mach, and all your G-code still works properly. So once you have working G-code, there's no reason to ever regenerate it, unless you actually change the design. Whether that's worth the change is up to you.

Regards,
Ray L.

[pete from TN]

That is basically it. I dunno about fudging anything as it does everything pretty much automatically. That is once the tool table is setup in sheetcam. I do not have a tool table for every program I run, rather a complete set of tools that do the lions share of my machining operations all setup and ready to go. When I do have an odd size to machine mostly drill bits I have a drill bit tool number that does not have an offset so it is like a generic tool. I usually try to make that my last machining operation or operations so I do not have to rezero my test tool twice and have only had to do it once or twice. Basically, I do the cam work using the tools with offsets, then start machining the part going thru each operation and toolchange when the program prompts it. Then when I get to the last one or two non tool length adjusted tools I just Zero on the surface with the tool and hit go. I also put a little text into the G code in sheetcam to remind me to rezero with that tool just in case. It would be nice to have a boatload of toolholders here but right now I only have like 26 I think. However that seems to be enough to do MOST of my projects as I usually call up my 1/2 and 3/8 three flutes for most of the roughing passes and then either my 1/4 or 3/16 two flutes for the inside tight corners stuff.... I also have a larger rougher or two if I need to get real nasty.... The rest are either champfer, drill, countersink, or some sort of measuring tool in the holders.

Like I said in my last post if and when I manage to break or damage a tool, I usually replace it IF I have one and zero it with the test tool, set my length offset for that particular tool and then manually set the length of the tool on the vise top or table top to whatever that offset is supposed to be. It does not take more than a few minutes usually...

I have been seriously looking at building some sort of toolchanger especially after seeing Tormachs TTS toolchanger prototype and I am sure at that point I will need to have tools setup in Mach and learn how to setup the axis for tool position. Much to do before then tho.... peace

Pete

[SCzEngrgGroup]

Pete,

If you try to do a TTS toolchanger, I think we've talked about the drawbar tension necessary to hold the tools with a machine the size of yours. I've come up with two ways of dealing with that: First, is a stepper motor, with a planetary gearbox. I've looked into this, and it would easily get you up to the 25 ft-lbs tightening torque necessary to achieve the required tension, with no Bellevilles. It would also give up to about 75 ft-lbs for loosening.

Option two is a pneumatic/hydraulic system. If you look at Harbor Freight, they have a very compact 10,000 pound short throw hydraulic cylinder for $20, and a pneumatic "multiplier" for, I think, about $60 that will generate 3,000 PSI hydraulic pressure from a 100PSI air source. That would allow you to do a Belleville drawbar if you wanted to. I prefer the stepper/gearbox solution myself, as it could easily be setup to loosen a turn or two to allow Tormach tools to drop out, or fully unscrew the R8 holder, so you could swap in non-Tormach tools.

When I retire in a few years, I'll get back on that project. But, since I went back to work in Feb, I haven't so much as turned on my mill...

Regards,
Ray L.