Hello all,i have just purchased a new HAAS toolroom mill tm1p.

i have decided to purchase the machine as i have had bad experiences with outsourcing some items we manufacture.

the bad part is i dont even know how to operate a cnc center, and i am just learning how to use entry level cad software,,emachineshop.

can someone please give reccomendations as to classes i can take for learnin g or cad software that will get me up and running quickly until i can learn how to use something like mastercam or pro engineer?

i live in Matthews NC right outside of Charlotte.


thank you

I'm barely 4 months ahead of you with the same machine. I would suggest the following;

Programming CNC Machines by Ken Evans
CNC Programming Handbook by Peter Smid

A Google search will bring up many sources. I think I used Amazon.

Call OneCNC (877-626-1262) and buy their CAM software. They have great phone tech support, a wonderful forum where you can post files you are having trouble with and experienced users will fix your problems, explain what and why they did what they did and then post the corrected file back on the forum. There are no annual fees involved, just the very reasonable up front cost. (reasonable compared to their competition)

You can also go to their web site ( OneCNC.com ) and down load a demo package at no cost.

My only connection to them is a hole in my check book. :)

Vern

070725-2131 EST USA

timmydabull:

Get the HAAS manual and study it. Geof will somewhat disagree.

If your machine is not available yet ask for a manual now, and/or go to the dealer and study the manual with one of their machines.

Power on is easy.

Next you need to home the machine. That is easy too.

Learn about the various screens and what the buttons do.

Learn how to write G and M code progams.

You need to make some decisions such as English/Metric, HAAS, Fanuc, or Yasnac mode. I suggest HAAS. Sign senses. RS232 parameters. And others.

You have to set tool parameters. On current machines G54 is selected automatically on power-up. You do not need a tool loaded to play. Learn how to move around manually, set rapid at 25% to start, set increment to 10/1000" to play with manual moving of the table, get a sense of table direction motion relative to the hand wheel, no need to play in MDI you can do the same things in an O-number program, learn to send and receive programs via floppy and RS232, and lots more.

You really need a good understanding of G and M coding before working with CAD/CAM.

.

070726-0557 EST USA

timmydabull:

Any program you write will have a structure like this:

%
O0054
(Desirable to have a comment here that identifies what this program is and/or does.)
(That is probably more characters than allowed in one comment on one line.)
(The left and right parens are the delimiters around the comment.)
(In the past you could not put a % in a comment because it would terminate program loading.)

Next you put all of the startup G-code required at the start of the program here.

Here you put the meat of the program.

M30 (You usually end the program with an M30)
(This stops the program and moves the program pointer to the first line of the the program.)
(The program does not restart until the next push of the start button.)
%

The %s are not stored internally in HAAS but are required in your file. You can put any junk in your file before the first % and HAAS ignores it.

The first % tells HAAS to start loading the program. The O-number is the internal name used by HAAS to find your program. You have no other way within HAAS to identify a program.

The second % found in the file being load terminates loading. In older machines a % anywhere in a file, including within a comment, would terminate loading. In newer machines HAAS has corrected this comment bug.

In my opinion for % to be used as a start or end delimiter it should be the first character following a CR or LF, but I have not tested a new HAAS for this.

If you want to load multiple O-number programs with just one operation of the RS232 RECV button, then put all the O-number programs in one file with one start % and one end %. This means no %s between the programs in this file.

.

070725-2131 EST USA

timmydabull:

Get the HAAS manual and study it. Geof will somewhat disagree.
......

Oh I don't know. I am not that sceptical of the Haas Manual :) . I did teach myself programming using primarily Haas manuals.

Don't be surprised if it seems difficult to understand, some stuff is not presented as clearly as I think it could be.

There is also a link somewhere in a thread on the Zone here to some pages about G code from Purdue University, I will try to find them.

timmydabull, i sent you a PM.

I don't know about others, but purchasing a few blocks of machinable wax was the best thing I could have done to teach myself CNC machining. While you can still break small tools, it takes a bit of pressure off the learning experience and then you can reclaim the wax to try again. Take a look at mcmaster.com, they sell a variety of high quality freeman waxes.

I learned G-Code programming from the HAAS manual. Dry reading but informative - the caveat is I am already an experience computer programmer. I learned the basic commands and went straight to CAM. I saw no point in messing around with coordinates too much as long as I knew what the commands were.

Thing is, there is so much still to learn. But that's half the fun. :)

thank you guys very much for your replies.
they have been very helpful and i will start with the advice all of you have given me.

the machine is to be delivered in the next 10 days so i am sure you guys will be hearing more from me soon.

thanks
tim

Here is that link I mentioned.

http://technology.calumet.purdue.edu/met/mfet/275/

There are a number of pdf pages you can download.

Hi Timmy :)

I bought a tm1 nearly 2 years ago , IMO spend a month(or less) or so getting used to the commands on the machine and a bit of quick code , then get Onecnc even just the 2.5 D package and get your TM smacking parts out ,how it s meant too!!!! (and connnect with RS232 cable:idea: )

Even if im drilling a couple holes ill send a onecnc prog to the machine, it just so easy with speeds and feeds all calculated.

All i do manully on the machine is blocking up really.

Cheers Kev :cheers:

Geof
thanks for the link.

Kev
will do
cheers

This might be a thread high jack if so I can move it but I think timmydabull might find it useful..

This is something that I have been thinking about for some time and I just responded to a post where the guy had some trouble with a positive number in the tool registry.
Geof you said in your response that you didn't use a cad-cam system.:eek:
I have found that a amazing amount of people program standing in front of the control.(chair)
I for the life of me cant understand why this would even be an option to anyone...please enlighten me:wave:

This might be a thread high jack if so I can move it but I think timmydabull might find it useful..

This is something that I have been thinking about for some time and I just responded to a post where the guy had some trouble with a positive number in the tool registry.
Geof you said in your response that you didn't use a cad-cam system.:eek:
I have found that a amazing amount of people program standing in front of the control.(chair)
I for the life of me cant understand why this would even be an option to anyone...please enlighten me:wave:

I am not going through the whole reason because it is all explained in a lot of posts in a lot of threads on the topic of hand coding versus Cam.

There are reasons:

One is that when I taught myself G-coding to move my business from totally manual production to CNC it was more efficient to do hand coding rather than spend months learning CAD/CAM. All the parts were designed and being made manually so hand coding was a snap.

Another reason came apparent when I had a guy who did do CAM; the programs run slower, sometimes a lot slower. We do small scale production anywhere from 10 to 2000 parts per batch and the batches repeat every three months or so. Even a few percent difference in cycle time can add up to a significant difference in total batch time.

Yet another reason is that when I design a new part I do not do it using CAD I do it on the machine and develop the production tooling at the same time. This way I make the initial protoypes on a simplified version of the fixturing that will be used for the production volumes and if I have to tweak features to enhance the efficiency of fixturing I can.

If you are only doing one-offs and if you take in outside work that has been designed by some nit who does not have a clue how things are made you are probably better off. indeed you probably have no choice, to use CAM. My situation is not common.

Didn't think that it was a sore subject..certainly not a right or wrong thing ..more of just a topic to talk about.
Sounds like you have it whipped no reason to change now

Didn't think that it was a sore subject..certainly not a right or wrong thing ..more of just a topic to talk about.
Sounds like you have it whipped no reason to change now

Some people got quite agitated telling me if I didn't have the smarts to use CAM I didn't have the smarts to run a successful business. It was quite amusing really but at the same time informative.

I think your 'certainly not a right or wrong thing' in some cases may not apply. I think the right thing is to maximize how much money your business makes and the correct way to calculate this takes into account all the time spent from when you first think about or look at a part to when the very last part comes of the machine. (I know I am repeating myself from other threads/posts here :) )

For prototypes and short runs the right way to minimize this time might be, probably will be, to use CAM.

For repeat or long production runs the right way to minimize this time might be, probably will be, to use hand coding.

If a person has never done hand coding and does not know how to do it effectively, and when it might be the right way, they are throwing away a potential competitive advantage.

070730-1422 EST USA

When you learn to hand code with G, M, and MACROS you learn the most fundamental commands that the CNC will respond to. This is equivalent to assembly language programming of a computer.

Any CAM program has to work with these codes, and almost certainly only works with a subset of these instructions. Therefore, the CAM system has to synthesize some functions from basic simple operations.

Here is a typical combination CAD/CAM problem. A designer creates a part with arcs, the CAD program outputs arcs as a sequence of short straight line segments. This propagates thru the CAM system into the CNC code as short straight strokes. Probably undesirable.

Suppose I have a block of material 12" x 12". Out of this I can make 36 indentical parts. I have multiple tool changes and various two axis contours. Also I want to face the whole top surface efficiently. In addition my stock is not always this size. I want a program where at the beginning I can specify the starting sequence position and how many to make. Obviously I want to minimize tool changes and this means select a tool and do all the required parts, then select another and so on.

This is hard, if not currently impossible, to do in a CAM system. But I can certainly make good use of the CAM system to do some of my program creation.

.

this is some very informative reading.
thanks

this is some very informative reading.
thanks

Here is some more.

I think fixturing skills are as important, sometimes more important than programming skills. Here is one fixture I recently developed:

http://www.cnczone.com/forums/showthread.php?t=38283

Here is a discussion I got into on the topic of hand coding versus CAM.

http://www.cnczone.com/forums/showthread.php?t=21953

If you get the impression reading this link that I am being deliberately provocative you are correct; it is a good way to get people to respond. I don't mind people disagreeing with me but I do like to see their reasons.

Here is that link I mentioned.

http://technology.calumet.purdue.edu/met/mfet/275/

There are a number of pdf pages you can download.


Geof, i am finding this link extremely useful and educational.

i have only read 6 of the lectures and it is bringing me up to speed quickly.

thank you very much.

The original source was mrainey I think so I can't take very much credit. I have read through some of them and they are indeed helpful.

Geof, I disagree wholeheartedly but I have to go to sleep so I Will get back on this tomorrow.
Joe

Suppose I have a block of material 12" x 12". Out of this I can make 36 indentical parts. I have multiple tool changes and various two axis contours. Also I want to face the whole top surface efficiently. In addition my stock is not always this size. I want a program where at the beginning I can specify the starting sequence position and how many to make. Obviously I want to minimize tool changes and this means select a tool and do all the required parts, then select another and so on.

This is hard, if not currently impossible, to do in a CAM system. But I can certainly make good use of the CAM system to do some of my program creation.

Gar, I can do this easily in Feature CAM. They have a very good method of dealing with multiple fixture offsets or multiple parts machined out of one block or multiple parts held in a fixture. You basically create one cam file with all the features you want machined. You then create a different file and specify whether your using individual blocks of stock, like in a fixture, or one big block. They also have different filters like minimize tool changes, or machine one part complete then move on to the next, minimize rapid distance, do finish cuts last, you can use the filters to adjust the automatic ordering or you can order everything manually.

Here are a few pics of a part and fixture I programmed with feature cam.

http://www.ewwenterpriseinc.com/images/BR215A.JPG

http://www.ewwenterpriseinc.com/images/BR215B.JPG

The part has two steps. The first pic was taken after the first step. I don't have a pic of the second step. I face the second end and cut a slot in the part in the same fixture.

070802-1935 EST USA

Ed:

I was trying to imply that you could not from a current CAD/CAM system generate a single program that you change a couple numbers at the machine in that single program and control the starting point in the matrix and the number to make.

One of my typical applications is X number of parts in a single line. Checking the first part I want to start at position 1 and machine 1 part. Then check it and maybe modify something in the cutting program. Next run 1 part at position 2. If this is good, then run X-2 parts starting at position 3. For production, then run X parts starting at position 1.

.

Geof, I disagree wholeheartedly but I have to go to sleep so I Will get back on this tomorrow.
Joe

I have to ask, which of the four do you disagree with? :)

The original source was mrainey I think

so I can't take very much credit.

I have read through some of them

and they are indeed helpful.



I hope it is not more than one of them.

Gordon,

I can do exactly what what to do except for the part about standing in front of the control to do it.

The part in the pics is one program for one single part. I can then, sitting at my desk instead of at the control, specify where I want the zero I programmed in the single part cam program. I can also specify repeat x times in x at a spacing I specify and repeat in y at a spacing I specify.

I can run one part in the fixture, check it, mod the cam program if needed, then run part two, check it, then run part three to whatever. I can then setup to run from part one to whatever on the second round all very easily.

Keep in mind I have very limited experience with macros, simply because in my chosen path to get the part programmed I don't feel I need macros yet. FeatureCAM does support macros and what your saying might be possible in the exact way you want to do it, but I don't know for sure, because of my lack in experience with FC and macros.

I do agree macros can be very powerful. My new okuma relies on a macro to tool change. I call the g111 macro and it checks what tool is in the spindle and omits the toolchange if the specified tool is already in the spindle. BTW this causes an alarm on an okuma and was very aggervating before I learned about the macro. It also prestages the next tool automatically. Very handy for one g-code. I also have one written to send the head up and back and center the table at the end of the program to simplify part loading. This works great to minimize the ammout of code that would be the same in each program.

I have read the post geof started about hand coding vs cam. Having used master cam V8, and owing a seat of OneCNC XR2 mill expert, and FeatureCAM Mill 2.5D, I think there are a few things you and geof are overlooking.

Not all CAM systems are created equal. A generalized statement about CAM system's programs cycle time being longer than a hand coded program's doesn't hold any weight. Especially in simply programs which has been the focus. An example was given where there was some drilling and boring, a simple program. There was also a statement about how the hand coded program would be faster. Both my cam systems allow me to use the same canned cycles for spot drill, drill, bore, etc. as you would use in your hand coded program. Both my cam systems will allow sorting of the operations so I'm not waisting time rapiding all over the place. Both systems will allow me to specify clearance and rapid planes. So where do you guys think a hand coded program will have any cycle time advantage?

Right now I have both my mills set up perfectly. They are connected with an I232 system to my cam computer. Both my posts are working perfectly for FC and I have OneCNC working perfectly on my Fadal. Haven't had time to get it working on the Okuma yet.

This was not always the case and I had to do some editing here and there. A lot of the time I would hand code and cut and past the hard toolpaths from cam. I agree that if you don't have you post perfect and you're not using the correct CAM system for the job, you might be able to program and run the job faster, but if you have everything set up correctly and are using the right cam software, watch out!

070803-0802 EST USA

Ed:

Since you use our I232 system you can send a 1 meg file at 115.2 kbaud in about 1.5 minutes. Thus, loading a large program is not much of a burden.

But for the person that is unfortunately at 9600 baud this 1.5 minutes turns into about 20 to 30 minutes. So in the case of the hand coded macro program there is very little time spent in program transfer vs the CAM program.

There are a number of tricks to minimize program size, minimize tool changes, and allow variable starting point and number of parts that can be employed when hand coding.

Sometime I will have to look at what FeatureCAM can do with macros.

As I believe you know HAAS can skip tool changes when the program calls a tool change and the tool is already loaded. This is inherent in their basic program rather than thru the use of a macro. There is a parameter or setting somewhere that determines how HAAS treats tool changes.

.

I do use your system, but unfortunatly my okuma will only communicate at 19,200 and my fadal will only communicate at 38,000.

I had a TM-1 and the baud rate was 115K along with my two haas lathes.

Toolcalls also worked fine if the tool was in the spindle on my Haas TM-1 and on the Fadal. It was one of the many things I had to get used to on the Okuma.

I still hand code the lathes and add the hard contours into my program because I haven't fully integrated the cam system with the lathe. When you have your post right and you've used the cam system long enough with the machine to trust it this is a huge deal. This is what I'm gettin at. Once everything is set up correctly, get out of the way!!!

.....I still hand code the lathes and add the hard contours into my program because I haven't fully integrated the cam system with the lathe. When you have your post right and you've used the cam system long enough with the machine to trust it this is a huge deal. This is what I'm gettin at. Once everything is set up correctly, get out of the way!!!

You comment about me overlooking things but you have not read my posts on the topic of Hand versus CAM.

First the thread you refer to was started by someone else.

Second if you look at my posts you will see that my main focus is that the advise CAM users give to novices to not worry about learning G code is wrong, wrong, wrong. I do not say don't use CAM, I do say for a lot of stuff you can probably do it quicker, and read my definition of quicker, by hand coding. I say that you need to know hand coding even if you now only use CAM and if you think about what you have written you are a perfect example that this is correct. You integrate CAM and hand to get the most effective use of both.

I will admit that I have expanded beyond just saying learn hand coding and have gone into justifying why I did not bother learning CAM. This has been mainly because I was dumped on by different people because I am so backward. It gets a bit tedious after a while being told I don't know what I am doing; how many people on this forum have installed 17 new machines in their shop in the past seven years paying cash for every single one with the 18th one currently in the quote stage. If I don't know what I am doing I am sure doing the wrong thing the right way.

End of rant.

070803-1212 EST USA

Ed:

I forgot your Fadal max'ed at 38.4. Does Okuma have an option you can get for a higher baud rate? If they have a 422 option at a higher rate we can probably work with that as well.

Those reading these comments should realize that when I use the term hand coding that I am not really talking about manually writing all the code, but rather putting together program components that make optimum use of the basic machine language (G, M, and macros). So mostly I would generate tool paths automatically from a drawing, and hang these together with appropriate logical structure for the goal at hand.

.

Hey Geof, I'm not trying to bust your balls, you can do it whatever way you wish. I've gotten good advise from you in the past, just trying to help you out now.

You misunderstood why I hand code the lathe. The only reason I still hand code to the lathe is because I still haven't gotten everything working perfect. Once that happens as it did with the mills I will never hand code again, unless your standing by the machine with a gun to my head :)

Gar, the okuma doesn't even dnc as standard equipment. That option is 4k to dnc with the 19kbps rs232. for 5k I got a data server from them with an onboard harddrive that the program can run from and eithernet, they have it installed but the tech didn't know how to work it, so I'm waiting for the applications engineer to show up and get it working. Doh!

Hey Geof, I'm not trying to bust your balls, you can do it whatever way you wish. I've gotten good advise from you in the past, just trying to help you out now....

Honestly I don't need helped out I am doing just fine doing things in my business my way. If I thought that spending several years becoming proficient in CAD/CAM was a good business decision I would do it.

If you do want to be helpful be helpful to the novices and make it clear that you do know manual G coding, that it is a valuable skill and that having a good knowledge of manual G coding allows you to utilize the CAM software to its greatest effect. In other words that it is a skill worth learning!

It doesn't take several years to be able to program parts. You probably would be able to program your first part in a few hours providing it's not a mars rover wheel or something like that.

I do know manual coding. I learned just like you. I was a manual machininst and bought my fadal used without knowing anything about how to program g-code. I learned by reading the manual, asking questions, and reading lots and lots of other peoples posts. That's the same way I learned cam software. If your able to teach yourself g-code and your obviously able to use a computer, you should have no problem with the cam software. I also believe you can't get anywhere if you don't understand the code, but if I have to take a math test and I'm offered a calculator, you bet your *ss I'm going to use it.

Btw, I was able to program your impeller from start to finish in 10 minutes. Your dimensions made it easy :) I replied to the other thread where you posted the "pepsi challenge"

It doesn't take several years to be able to program parts. You probably would be able to program your first part in a few hours providing it's not a mars rover wheel or something like that.....

I think you have a higher estimate of my abilities than I have :) . I have had various people give me guesstimates of how long the learning curve would be for someone knowledgeable in machining but a complete novice when it comes to CAD/CAM and the most beleivable one came up with about eight months.

Actually right now, today, if I was faced with the question whether I should learn CAD/CAM to convert my company fully to CNC from all manual machines I do not know what the answer would be.

You must take into account that this decision was made in 1999 and early 2000. CAM programs have advanced dramatically in the past seven years so doing a comparison now is not relevant to the situation that prevailed back then.

Also back then I did not know manual programming so I would have had to learn it anyway in order to progress into CAM. It was simply more efficient to just do things manually once I had developed rudimentary programming skills. Now it is more or less pointless for me to learn CAM; I am a few percent retired now with the percentage gradually increasing. If my company needs more CAM expertise than is available already on staff I will hire someone.

You said it the other thread you have someone at your shop that does cam programming, this is what you were compairing the cycle times too. What cam system is he using?

You said it the other thread you have someone at your shop that does cam programming, this is what you were compairing the cycle times too. What cam system is he using?

That was one comparison, another was a student at our local tech school took one of our parts and they programmed as a demo, yet another was the impeller I posted in the other thread. The hand coded program runs about 15% faster than the program from ONECNC for the complete part with all three tools. Your program had only one tool for the initial roughing, it uses a 0.525" DOC and does not leave the step at the bottom for the fillet. It runs faster than the first tool in the hand coded program because the hand coded one uses 0.35" DOC and has an extra sequence to leave the step for the fillet. When the hand coded one is edited to use 0.525" DOC and omit the passes for the step it runs faster than your one.

I think my guy use MasterCam which he brought with him when he joined us. We only used it for engraving on arcs until I found out it was pirated so I told him to get it off the company computers. Now he does the arc engraving using Macros.

I forgot about the fillet. Did you want the fillet on the bottom and the top edge too? Do you want a through hole in the center?

I didn't tweak anything, yet. I would go the whole 1.05 Doc with the SGS S-CARBS I use :) and change the stepover a little. I think this style of programming would be harder for you. There is more code that needs to be written for the smaller stepover with less z levels, vs the wider cuts with more z levels because you can copy what was already written and edit the z.

If you want, you can download the free FeatureCAM demo and I can walk you through the steps needed to program the impeller so you can see for yourself how well it works.

You mentioned you use a simple cad program to figure tangent point, etc. Which program are you using? I think your further along on the path to learning cad/cam than you think. If you can already draw basic shapes and have been using cad your halfway there.

I forgot about the fillet. Did you want the fillet on the bottom and the top edge too? Do you want a through hole in the center?
.

This impeller is not a product it is just a programming exercise that I did for fun one Friday afternoon when I was feeling bored. There was this thread about designing an impeller:

http://www.cnczone.com/forums/showthread.php?p=105391#post105391

I followed the posts and here are two quotes from different posts:

One of the first trys dry verified at about 120 hours to do the job. By roughing out the major pocket with a 1/4" and then doing outside offset of each vane with a 1/8", it got the whole process down to about 2 hours. Along the way, I tried various offsets etc. This is the beauty of Cam, I can make a change and redo the entire gcode in a few minutes. Try doing that by hand and it could take days to complete.

Well, I stayed up all night last night and put the file below together. It's a G-code file for an impeller with seven vanes and 1 inch across.

My first though when I read these is not typable for polite reading.

So being bored I did the impeller, took some pictures and posted them in post #15. I did not keep a really good track of my time but from first thinking about doing it to the final thing that I took pictures of was between 4 and 5 hours. And that included hogging the big piece of scrap down to get a 4" diameter.

This first attempt just did the single tool and did not leave material for fillets and that is how I left it. I'd had a bit of fun, overcome my boredom and proved that I was a hell of a lot faster at hand coding than some people are with CAM.

Then I got involved in the discussion in the thread about CAM for a Haas. My contention is that to effectively utilise CAM you need to know hand coding and also if you are doing production and the part can be hand coded it probably should be hand coded because the program will run faster.

So I went back to my impeller and spent about 30 to 60 minutes putting in the other tools for the fillet and top radius and posted this as a good program to do a comparison between CAM and hand. Obviously it was possible to hand code it, however, these days most people would not dream of it. I posted the key dimensions so anybody could replicate it in a CAD/CAM program.

As a side comment you said it took 10 minutes to draw from my dimensions/coordinates. How long would it have taken you to start from scratch with only an idea? Remember in my first 4 or 5 hours I have the original design process included; that took more than a few minutes.

I haven't look back but I think there were a couple of programs posted for me to compare, one was very slow and one very good and then yours.

And that is where I left it. I knew my program ran faster than a CAM program and the only thing to consider was how many parts had to be run. The break point was a couple of hundred or so.


I didn't tweak anything, yet. I would go the whole 1.05 Doc with the SGS S-CARBS I use :) and change the stepover a little. I think this style of programming would be harder for you. There is more code that needs to be written for the smaller stepover with less z levels, vs the wider cuts with more z levels because you can copy what was already written and edit the z.
.

Go and look at my program. All the vane coordinates are in subroutines, to change the Z step is just a matter of adding or removing subroutine calls. It took about 15 seconds to edit the program to your DOC and take out a finish pass so yours and mine did the same amount of work. Also to change the amount left on for a finish cut is determined by the D11 tool diameter. I often use two or more tool diameters so I can use the same set of coordinates for roughing and finishing.


If you want, you can download the free FeatureCAM demo and I can walk you through the steps needed to program the impeller so you can see for yourself how well it works.
.

Thank you for the offer but I wish I could convince you I am not going to bother learning any CAM, at least not at this stage. As I say maybe in the future my company will but right now my main focus is improving productivity by designing and building multi-part rotary fixtures to complete operations on up to three sides in a single fixturing.

Perhaps you have already seen this thread:

http://www.cnczone.com/forums/showthread.php?t=38283


You mentioned you use a simple cad program to figure tangent point, etc. Which program are you using? I think your further along on the path to learning cad/cam than you think. If you can already draw basic shapes and have been using cad your halfway there.

The program I use is AutoSketch, about 18 years old and runs in DOS. I find it very hand to do quick 2D sketches and pull out tangent points. Sometimes it is tedious such as with the impeller example but if you take advantage of geometry and position things correctly you only need locate coordinates for one blade; everything else comes from switching +/- and X/Y.

I do know how far along I am in CAD and I do know if I put in a few weeks of intensive study I could master any CAD program. You must remember though that I am also running a company. I spend a lot of time amusing myself on CNCzone because these days I have people to do the grunt work, and not so grunt work, but I am needed to make decisions and do the detailed stuff and it is impossible to learn something technical if you get disturbed every hour or so and have to switch your mind to something else. Also if I am going to be away from day to day operations I would much rather be sitting in the bar on a cruise ship relaxing.

Go and look at my program. All the vane coordinates are in subroutines, to change the Z step is just a matter of adding or removing subroutine calls. It took about 15 seconds to edit the program to your DOC and take out a finish pass so yours and mine did the same amount of work. Also to change the amount left on for a finish cut is determined by the D11 tool diameter. I often use two or more tool diameters so I can use the same set of coordinates for roughing and finishing.

I did look at your code. I don't have nc plot so all I could really do is "look" at it. I understand what a subroutine is and how you called each one. This is in essence copying the first toolpath and repeating it multiple times. This is basically what I said you were doing. I don't think you would be able to cut the part at the whole depth of cut or even .525 Doc. Why because I'm taking a .1665" stepover, I could take the whole depth of cut and reduce my stepover. This way I can use the full length of my carbide endmill's flute. I'm not plowing through the part at 100% cutter engagement anywhere. Sure on internal corners the % engagement increases but FC automatically adjusts the feedrate for the corner. It also increases the feed around outside corners.

(edit) FC automatically adjusts the feedrate for finishing. For roughing you must specify feed rate optimization. This will increase or decrease the feed rate based on a target hp for the tool and what the material removal rate is at each instance in the toolpath. I don't know if this would be benificial for aluminum, but I bet it comes in pretty handy for harder to machine materials. (end edit)

This is what I was trying to say. It's too hard to write the toolpath to take many smaller cuts, it's much easier to take bigger cuts. This leads itself to your method of many z increments because it's easy to write. You also can't change the stepover easily to experiment. Cam gives you a lot of flexibility with the code.

I added the radius at the bottom, no big deal. Since I left .050 for finish I just had to change the finishing tool to a .5 endmill with a .030 raduis. A few second fix, and add one toolchange to my cycle time.

I honestly don't know how long it would take to design such a thing. But I do know if I had to hand code it you would have me beat :)

You said you have 17 or so machines in your shop with one more possibly on the way. Are they all cnc's, or are some manual?

Are you the only one that programs in your shop?

Sorry for all the questions just trying to get a feel for the situation.

.....You said you have 17 or so machines in your shop with one more possibly on the way. Are they all cnc's, or are some manual?

Are you the only one that programs in your shop?

Sorry for all the questions just trying to get a feel for the situation.

All Haas machines. TL1 being modified for tubing parting and finishing, I started a thread on this, TL1 used mostly for making fixtures, GT20 used for bar work up to 2-3/4" diameter, HL1 used for bar work up to 1-1/2" diameter with air over hydraulic barfeed, HL1 Big Bore used for bar work up to 2-1/4" barfeed not finished yet, two SL10s with hydraulic barfeeds used for bar work up to 1-3/8" dia., two MiniMills, three Super MiniMills, three VF2s, VF0, GR510. Plus a manual mill and lathe.

I did most of the programming. I have 3 or 4 guys who can program but that is not their main function. I am the one who develops new products and does the programming and fixture design but at the moment one guy is working almost full time on making the new rotary fixture tooling.

You won't give up trying to convince me how wonderful CAM is will you :) .

Wow, that's an impressive list of machinery. With all the $$$'s in machinery you have a 2.5d cam systems price is like a drop in the bucket. IIRC I paid around 3k for the FC basic 2.5d system that also had 4th axis positional included as standard equipment. They were running a deal at the time, if you owned another cam system, I had OncCNC, they would give you a pretty good discount.

Do you use software in other areas of you shop? I use Quickbooks and wouldn't even dream of trying to do all that accounting BS on paper. I also use E2 Shop System to run the shop. It's also very effictive at lowering my stress level :) I planning on adding barcode data collection to the system so I can track employee productivity.

070810-1023 EST USA

Ed:

Would you mind visiting the Fadal thread
http://www.cnczone.com/forums/showthread.php?t=41741
and describe the details of the problem you had before you contacted me?

There may be some similarity.

.

Guys, i just got the new machine up and running,tried to do the spindle warm up but couldnt get the program to load and execute.

i will be studying the manual the rest of the day.

thanks for all your help, heres pics of the machine

Nice! Really wish my employer had bought the enclosure. It makes a mess otherwise.

First thing I do is turn off the safety switch override. The spindle warmup won't run otherwise unless I am there holding the button and I don't want to do that for 20 min. This is in the settings menu, just push pgdn until you find "Safe Switch Override" Then change to "on" and hit enter then Y. You may not have to do this on a TM-1P though.

As far as running, go to Prog List, find the warm-up program select it and press enter. Then you can hit cycle-start from there or go to the current commands screen to see your feed and speed. You can hit cycle start from either place. Be sure to set the rpm override for the warm-up program for your machine. It's 50% for my TM-1, so I am guessing 75% for yours since it is 6000rpm.

Have fun. :D

i am getting the wrong section error, i guess it will take more reading of the manual.....

thanks

"Wrong section error"? Don't think I've ever seen that one before.

im sorry i cant think of the term for some reason something about the manual mode the midi button seemed to take me further along.

then i started getting zerox and zeroy errors i guess i need to find out how to set those.

oh well i will get back to this topic once i get half an idea what im doing,,until then thanks.

070812-1019 EST USA

timmydabull:

I think you should start a separate thread for your questions.

It is not clear what you are saying and I am not familar with your particular machine.

However, following is a general bit of information.

Turn power on. Make sure you have air pressure. There should be an error message if air pressure is low.

You should have some sort of alarm. Push RESET button.

Push POWER UP RESTART. You will probably get an alarm relating to door closure. Close the door. Try again. Instead of this we go to settings and page down to Door Hold Override and right cursor once to ON, then push WRITE. Now the machine will run with the door open. It is your responsibility when you override the door switch.

Push POWER UP RESTART and the machine should automatically and slowly go to machine home. This is a great convenience in comparison with some of HAAS's competitors. The home position is with the table to the extreme left and toward you, and Z at tool change position.

Push the HAND JOG 0.01 button. Push one of the axis buttons. Now the handwheel will move that axis in 0.01 increments per handwheel pulse.

Can you get this to work?

.

There is one addition to gar's list. On the Toolroom machines after doing the Power On, Reset, Move Door, Auto Restart the machine will stop with a screen that reads Manual (something) in large red text. Now you push Write and you can then push Handle Jog and move the axes manually.

In Handle Jog if you get a No Zero X, Y or Z that means you have not done the Auto Restart.

If you get a X, Y or Z travel exceeded in MDI you are trying to make the axis move too far based on whatever coordinate system is active.

Incidentally gar's advise regarding turning off the Door Interlock may not work on a Toolroom machine. It depends both on a Setting and one or more Parameters. If you are just learning it is much safer to leave the Door Interlock alone.

Push POWER UP RESTART and the machine should automatically and slowly go to machine home. This is a great convenience in comparison with some of HAAS's competitors.

I've only used a HAAS. What do the competitor's do on power-up?

070812-1150 EST USA

Thanks Geof for filling in information I am not familar with.

My reason for suggesting this be in a different thread is because it would be useful for someone starting without any prior background.

It might be titled "Starting to work with a HAAS".

When first starting there are some necessary decisions like ---
HAAS, Fanuc, and Yasnac mode, setting 58, etc.
Inch, metric setting 9.
81 Tool At Power Up.
83 M30 Resets Override.

This is just a sampling.

.

.....My reason for suggesting this be in a different thread is because it would be useful for someone starting without any prior background.

It might be titled "Starting to work with a HAAS".....

Why don't you take the honor of starting it :) . It could be very useful.

Gar, yes that works thanks

thanks Gar
it works now,i havent gotten the spindle to turn but i can manually jog all the axis.

i forgot to push the jog speed,and manual jog button before.

070812-1651 EST USA

Geof:

I am thinking about your comment.

timmydabull:

What specifically did Geof or I say that solved your problem?

I am going to suggest that you set up for HAAS mode, setting 58. You do this by going to the SETTINGS page, then to setting 58, right cursor to HAAS, and push WRITE. In HAAS mode if you are not doing anything with G52 put this line of code in every program before any motions:
G52 X0 Y0 Z0

When you get more comfortable with HAAS I will make some comments on how you might use G52.

When you write a program on your computer it must start off with

%
Oxxx
(a comment to tell you what this program all about)
your program initialization stuff
your program code
%

You have to start with a %.

The Oxxx is you program number that is used internal to HAAS. Oxxx can have 1 to 5 decmial digits for xxx on newer machines. Older machines are limited to 4 digits.

Comments must always be delimited by a left and right paren ( parenthesis), and there is a maximum limit between parens or maybe it is a line length limit.

You must always have an ending %.

When you load a program HAAS does not start the load until the line after the first (start) percent. It loads eveything until the next (ending) percent unless there is an error. It will wait forever without the ending percent.

.

he said to push the write/enter button in manual mode and to press the .001/100 button before trying to jog axis,i had it 85% but wouldnt work until i did those 2 things

%
Oxxx
(a comment to tell you what this program all about)
your program initialization stuff
your program code
%

You have to start with a %.



that makes sense,thank you

Hey guys just wanted to come back and give an update on my progress with the new machine.


after 3 or 4 weeks of working with the machine
i have gotten familiar enough to set tool offsets setup workpiece offsets and hand program some g code,even run a small batch of parts.

i wanted to personally thank all of you who have helped,your advice and the wealth of information on this site has been very helpful.

i am very greatful for your help.
thank you


now its time to start working with cad/cam
cheers

ok 6 weeks

ok 6 weeks

That sounds about right; it took me six weeks from getting a HL1 to actually getting a finished part off the machine. I had never done anything with CNC before.

In my opinion you should spend about another six months or more polishing your G code skills then start doing CAM

Geof, i will try my best to follow your advise,however all the machining projects i have form here on will be 3d stuff.