Programming for so many years on my own and wondering how the real world does it.

Programming for years on my own. Wondering how the real world does it.

What I've learned since reading these forums, is that everybody has their own way of doing things. And some of them very different from me.

A little background.

Even though I've operated a job shop for almost 15 years, I've never worked in another machine shop in my life other than my own. Everything has been self taught. That is why I'm here to, in a minute, ask others how they do things and with what resources. I'm a long time BobCAD user still using V21, because after trying and buying V23, I couldn't imagine anything getting worse, or being so bad at developing machining code, and drawing for that matter. Now I only use V23 for opening files that V21 has trouble with. And a few small other things. (I should note that I do only milling, and BC is at V28.)

98% of my programming is done off of 2D drawings. I select the tools, and when and how they run. I set all the feeds and speeds and DOC and the like. I use certain CAM functionality available in V21 like pocketing, helical path, and profile, which allows me to choose a part feature outline, tell the tool where to start and which direction to run, give it a lead in and out of my choosing and so on. Trust me, I'm not typing in any X or Y coordinates, or I's J's or K's manually at all. I do a fair amount of copy and pasting but little direct typing other then some M and comp or exact stop G codes, Z moves and feed rates, notes in parenthesis, and bring the table to where I want it for fixture work and reloading.

Questions form.

When you look into many CAM or CAD/CAM packages, you're usually dazzled with these amazing 3D part renderings with millions of fancy tool path lines surrounding them. I think the idea is that with just a few clicks you can create any complex part in a very short amount of time. After trying it in V23 many times and finding it mostly useless, one question I've developed is... does anybody actually use this stuff in real life? I can see using it for complex shapes that have few square corners or edges, like golf club heads or turbine blades or propellers, but for the regular stuff with standard geometric shapes and clearly defined boundaries? I mean many of my parts need over 20 some tools to produce. Do programmers slug through this type of process, paging through hundreds of menus and drop down boxes in a full 3D menu driven environment to get to a fully machined by multiple tools part? It's my understanding that these CAM packages are not capable of making all these choices on their own. Is that correct? Isn't it like any other computer in that it really needs be told everything anyway? (Accept coordinate points that the CAM easily fills in.)

(Keep this in mind as I ask my questions. I'm not here to argue over what package is better than the other. More so how much functionality do you use with what you've got. Or how much manual intervention do you use.)

I would love to own Such & Such, because it seems to be the professional's choice of software for machinist who make their living making chips. But the cost has always been way over my head. Though one of my questions is to ask... is it worth it regardless? Part of my questioning here is, have I been shooting myself in the foot all along by not using and paying up front for this type of high end functionality? And are there CAD/CAM packages out there that can truly develop small to medium run production part programs? Or are the benefits gained by their ability to visually back plot programs and check for crashes and gouging? Even if you do check this out in the programming stage, does anybody actually run these so called "tested and proven" programs first time through without the operator reading along with his/her fingers glued to the feed hold, single block and start buttons? If so, then were is the savings?

I await the communities help, because I'm concerned that being mostly on my own for so long has limited my scope of how the real world lives in the job shop programming environment. Thank you for reading.

David

David,
If you run production which is based on minutes and seconds per part, every advantage you can get is worth the cost because that's what keeps you in the business. Starting from machines which no longer are build as they were before. Heavy box way are replaced by lighter and faster leniar guides. They last e certain amount of years and than its time for newer and fasrer. it seems to me that you are it I this type of business and few minutes more per part doesn't really matter. Am I correct ? I think so, and I share the same perspective. My Mori Seiki is 30 years old and I have never run it at its full speed. I run things and I listen. if it's starts to complain I back off the a bit and it runs happy.
Tool paths and tooling makes a difference only when time per cycle is the bottom line. It is hard to argue which way is better , I like it my way and that's what counts for me. Machines are only as good as the hands behind it. If you you have to program and run few different parts per day , a good intuitive CAD/CAM will also benefit your opertion.
Let the machine and software work harder and you work smarter.
If it comes to running it right out of the CAM.
I do it all the time and learned to trust it. I can't help to keep my finger on the feed hold and over overnight knob but mainly to fine tune the feed rate more than anything else (for initial run of the part.)
I already know what the machine will do looking at the simulation, plotted from the code.
Is there a perfect CAD/CAM ? I don't think so but things evolve.

Regarding the cost , things like this are tax dedactible, it's cost of doing business same as tooling and electricity. If you are running your operation from small home shop it's hard to justify the huge price tag.
It all depends how you look at things and if moral aspect is not an issue.
Everything can be found on the Internet for free or much lower price.
SolidWorks can be purchased for a fraction of what it cost as a student or Veteran if I am correct.
Is it a right thing to go about it this way ? The answer may be very personal for everybody. If only few can afford the expense and the rest of as are out in disadvantage just because we don't have enough volume of the work to be able to afford a good CAD/CAM , then you do what you got to do to survive. If however you cheat and lie because your greed , well that's a different story.
Kind regards.
Mike.




Sent from my iPhone using Tapatalk

As Mike mentioned it really depends on whether or not you're a production shop or a jobbing how you approach programming. If there is a safer option that takes 5 minutes longer and you're only making a couple of widgets why try and break any speed records?

That said there are lots of times where the new tangled tool paths kick serious ass when it comes to roughing strategies. I can either spend hours drawing complicated geometry for pockets and walls and tapers and individually and lovingly select each one or I can draw a simple box, select the model and let my computer do the think in' and doin' for me. I'll let you decide which one I choose more often than not... I keep 5 guys busy full time I don't have time to waste.

As far as crashes avoidance goes, I trust my software, if it says it isn't going to crash and I have my fixturing and part modelled and set up correctly I don't worry about it. That doesn't mean the operators are careless walking away from the machine but the pucker factor is greatly reduced when you are reasonably assured nothing weird is going to happen.

I went from slugging it out the hard way with an old version of Bobcad to OneCNC, specifically because it couldn't, at the time, do anything with a 3d cad model. OneCNC was my first experience with a cadcam that had any sort of automation to toolpathing where you could show it the model and it would create the entire roughing and finishing toolpaths in two operations. It blew me away at that time how had I never had an inkling that something like this was possible, with software in the price range of a small shop budget.

I still prefer to use a 3d machining strategy at any time when there is some feature on the model that I need to not gouge into, but is a feature that is prone to getting gouged. For example, a generous fillet at the bottom of a pocket, something where the radius is larger than that of the roughing tool. I do not ever want to sit there and figure out how deep can I go before I have to watch the possible interference of the tool with that fillet. I just use a Z level roughing strategy, either a conventional or a high speed toolpath, whatever suits the situation.

Another scenario: machine two small parts in pairs at one vise station. Plop a second copy of the model down a reasonable distance from the first one. Use a 3d strategy to do the roughing around both of them: no picking profiles at this stage, just let the software do the work it excels at. Then, go to profiling to do the final finish on some important features.

It turns out, the 3d strategies that are 'model aware' are a very good reason to have a 3d cad model to begin with. The 3d strategies are the easiest to deploy. Your only decision is setting the parameters to do the toolpath in a reasonable length of time within the capabilities of the setup and the machine, of course. I only ride the single start button until I get the new tool down to the first clearance distance above the part. Then, it is auto from there on. I already simulated it and have proven it that way, there is little point in not trusting the code from there on. That is not to say that in some situations, you might discover that your machine post needs a bit of a tweak (let's say because you introduced a 4th axis). But in those situations, one is generally going slow or single step until you are dead sure that the tool is getting from home to the part in a safe manner and is rising to proper clearance between ops. This is more of a confidence issue with your own programming habits. Still, the simulation should show interference if you've got your wits about you.

David,

If you post a sample of how you would program a part, I will give an example on how program your part if you don't want to post the file on the internet. I would more then happy walk through it using gotomeeting or something like that

13engines,
I use FeatureCAM. FeatureCAM has a function called "automatic feature recognition" (AFR).
This is supposed to basically program the part for you (as you kind of vaguely described).
I gave up on AFR years ago.
In a great attempt to get this AFR to function in such a way that the software would create a logical machining strategy, and spit out sensible code.
I spent considerable time on my machine/tool defaults and attributes. This was not time wasted, because it helps immensely whether using AFR or not.
And, I still find myself tweaking attributes quite often.
(nevermind the fact that FeatureCAM can be "buggy" and change shit on its own! But, that is a different subject )
But, I never really did get acceptable results from AFR. I gave it a fair shake in the beginning. But, eventually learned, it was not helping me in any way.
By the time I would go in and tweak all the machining variables that AFR came up with, to get what I really wanted, I was time ahead to just not even mess with AFR.
I just quit using it all together, and probably have not touched it in at least 5 years.
The good thing for me is, FeatureCAM is a very quick software, so not having great AFR functionality, is no sweat off my back.

In a strictly production environment, I don't believe FeatureCAM is a great option.
MasterCAM (mentioned specifically, because I have experience with it) gives a programmer much greater control over tweaking tool-path.
In a strictly production environment, when every second counts, those perfectly tuned tool-paths are very important.
FeatureCAM is pretty intuitive. Which can be a great thing, and is part of what makes it fast. But at times can be a little too intuitive.
And, it is those times that it becomes very time consuming tweaking tool-path.

But, reading through your initial post, it looks to me like you have a pretty good handle on what you are doing.

David

A lot depends on how much you want to spend and what kind of work you do. I have been programming for 18 years now and over the course of time picked up a lot of new ways of machining. I work on single parts jobs and multiple part jobs in fixtures. Personally I think you will learn more and become a better programmer learning a new software package. I started out with smartcam first which was all wire frame/2d. I learned Edgecam and surfcam later on. Today I work with Camworks with is a good software package for what we run at our shop. There are a lot of expensive and inexpensive software packages to try out. I don't have a good answer which one is the best to try out but most of them are very similar on how they run. I like working with solid models and I design most of my fixtures inside of Solidworks. It is nice laying out a part and importing the hardware for the designs. This may be something you may like to see when programming. It may be worth your while to check out a few websites and call a few vendors for a demo of their software. send them a part you worked on and see how they can program that part.

If you decide to get a software package it will be tough at first and discouraging when you start using it because you can always fall back on the older package you are use to using. The struggles will slowly go away as you get more efficient and start discovering better ways of machining. You can also use the more current software package for quoting which I do a lot at my place.

13engines said:

What I've learned since reading these forums, is that everybody has their own way of doing things. And some of them very different from me.

A little background.

Even though I've operated a job shop for almost 15 years, I've never worked in another machine shop in my life other than my own. Everything has been self taught. That is why I'm here to, in a minute, ask others how they do things and with what resources. I'm a long time BobCAD user still using V21, because after trying and buying V23, I couldn't imagine anything getting worse, or being so bad at developing machining code, and drawing for that matter. Now I only use V23 for opening files that V21 has trouble with. And a few small other things. (I should note that I do only milling, and BC is at V28.)

98% of my programming is done off of 2D drawings. I select the tools, and when and how they run. I set all the feeds and speeds and DOC and the like. I use certain CAM functionality available in V21 like pocketing, helical path, and profile, which allows me to choose a part feature outline, tell the tool where to start and which direction to run, give it a lead in and out of my choosing and so on. Trust me, I'm not typing in any X or Y coordinates, or I's J's or K's manually at all. I do a fair amount of copy and pasting but little direct typing other then some M and comp or exact stop G codes, Z moves and feed rates, notes in parenthesis, and bring the table to where I want it for fixture work and reloading.

Questions form.

When you look into many CAM or CAD/CAM packages, you're usually dazzled with these amazing 3D part renderings with millions of fancy tool path lines surrounding them. I think the idea is that with just a few clicks you can create any complex part in a very short amount of time. After trying it in V23 many times and finding it mostly useless, one question I've developed is... does anybody actually use this stuff in real life? I can see using it for complex shapes that have few square corners or edges, like golf club heads or turbine blades or propellers, but for the regular stuff with standard geometric shapes and clearly defined boundaries? I mean many of my parts need over 20 some tools to produce. Do programmers slug through this type of process, paging through hundreds of menus and drop down boxes in a full 3D menu driven environment to get to a fully machined by multiple tools part? It's my understanding that these CAM packages are not capable of making all these choices on their own. Is that correct? Isn't it like any other computer in that it really needs be told everything anyway? (Accept coordinate points that the CAM easily fills in.)

(Keep this in mind as I ask my questions. I'm not here to argue over what package is better than the other. More so how much functionality do you use with what you've got. Or how much manual intervention do you use.)

I would love to own Such & Such, because it seems to be the professional's choice of software for machinist who make their living making chips. But the cost has always been way over my head. Though one of my questions is to ask... is it worth it regardless? Part of my questioning here is, have I been shooting myself in the foot all along by not using and paying up front for this type of high end functionality? And are there CAD/CAM packages out there that can truly develop small to medium run production part programs? Or are the benefits gained by their ability to visually back plot programs and check for crashes and gouging? Even if you do check this out in the programming stage, does anybody actually run these so called "tested and proven" programs first time through without the operator reading along with his/her fingers glued to the feed hold, single block and start buttons? If so, then were is the savings?

I await the communities help, because I'm concerned that being mostly on my own for so long has limited my scope of how the real world lives in the job shop programming environment. Thank you for reading.

David

Click to expand...

Virtually everyone is just about as isolated as you are, using one piece of software extensively, and either believing it's the messiah and/or satan. Either wishing they had the resources to buy something better, or believing everyone else is idiots for using anything different. None of them, regardless of cost, are anywhere close to perfect for doing everything.

Fusion 360, today, is $25 via amazon prime.

I told myself I wouldn't promote it..

But go watch a few videos on Youtube, then buy a $25, one year license.

The value proposition with $25 fusion 360 is so insanely much higher than everything else available ever, it's stupid that anything else even exists. It's like if a BMW 3-series went on sale every once in awhile for $200.

rlockwood said:

Virtually everyone is just about as isolated as you are, using one piece of software extensively, and either believing it's the messiah and/or satan. Either wishing they had the resources to buy something better, or believing everyone else is idiots for using anything different. None of them, regardless of cost, are anywhere close to perfect for doing everything.

Fusion 360, today, is $25 via amazon prime.

I told myself I wouldn't promote it..

But go watch a few videos on Youtube, then buy a $25, one year license.

The value proposition with $25 fusion 360 is so insanely much higher than everything else available ever, it's stupid that anything else even exists. It's like if a BMW 3-series went on sale every once in awhile for $200.

Click to expand...

It's free unless he makes over 100k in revenue

If you visit emastercam.com you can download the "home learning" version of MasterCam X8. It has the full functionality of the software, except posting of course. And any files you create in that version are unusable in other versions of MC.

If your parts are mostly simple square corner geometries, then what it comes down to is personal preference on the software's interface, buttons, icons, menus etc. A good test of this is to compare how many "clicks" it takes to make the same part in two different softwares.

As mentioned above, MasterCam has a TON of control on every little detail of your toolpath. Just the lead in/lead out page of a basic profile path has about 20-30 different options/buttons/settings you can mess with.

First thanks to all those that responded. I'm getting it that people really do use the 3D cam capabilities of their software. I also realize that I'm not going anywhere new until I get off this XP Pro operating system. Time for Windows 7 at least.

I should clarify that most of the parts I do have features that can be created with some form of standard tooling or a creative tool path. Many in vises or multiple twin vises. Many on fixtures I have to build. Once in awhile I'll get something that has curves that can only be created by some step over machining technique. My work ranges from fairly complex with 20-25 separate tools down to quick and easy and under 10 tools. Quantities from one or two up to 200. Most in the 25-75 range.

I ask to clarify a couple things. So my fellow programmers are selecting entire 3D models, selecting a roughing and finishing strategy, and in a minute you've got your program? How does one end up with 20 some tools? Or do you select each surface features and plow through each one while telling the software what tool and what step over to take and all that? I mean, after programming a complex part with many features and various chamfers, are you left with this large library of selected rouging and finishing strategies selected through your software, that together represent multiple tools creating multiple part features? What about drilling cycles? And do you as one person said, have to over time, develop very deep tool archives, so when you call up a tool, much of its values are already filled in? I'm still a tad lost as to what is actually accomplished in a nearly hands-off-and-let-the-software-do-it approach to programming.

The bit I wrote about first run gitters is because with my versions of BobCad, the resolution and quality of back plotting them over a solid model is practically useless. You can't see anything for sure.

I agree with what one person said in that trying other software will most likely expand my programming skills. That I can see. I'm looking to feel more competitive in the market, and I can imagine high end software could help me get there. As an aside, I've also nearly completed a ground up rebuild of a Mori Seiki SV-50 VMC with a pallet changer. All new screws and rails, bearings, you name it. It's a triple jump from where I am now in its speed and capabilities, both in hardware and control features, so I'm anxious to consider amping up my programming to take advantage of it. Also I'm nearly finished implementing a full 4th axis on both machines. Another unknown programming landscape for me to get hip on. Plus this new machine has probing and Macro B. I feel my plate getting very full in the programming department.

Again thanks everyone for taking time to respond. Highly appreciated.

David

Generally, a part takes as many unique tools as is required for particular features, no magic there.

Maybe for mold roughing (which is what I was attempting to do when I switched to OneCNC) a single roughing routine is all that is required to open up the cavity for finishing ops. But then you'd look for 'rest machining' options to automatically find and help clean up areas where larger tools don't fit and let the software both find and machine those areas.

There is plenty of room for you to use your own preferences and experience to machine with suitable tools. The software does not literally force nor volunteer that you use any particular tool.

So my general experience in 3d machining is that I spend time thinking about what tools I have available, and how I want to apply them (nearly everything seems to require tools that are too small a diameter and a ridiculous extension, and this requires strategy planning) and practically no time thinking about actually making toolpaths. I'll spend the time required to run a full simulation and view the model carefully for any gouge type errors that indicate some of my settings are out of wack. Always simulate is my rule, the stupidest things can occur sometimes and I feel pretty dumb when I jump the gun (don't sim), run the program, see the error and go back and simulate it, and 'yep' there it shows up alright. Self-kick!

Having taken the time to simulate, then I don't single step at the control any farther than to prove that I have set my work offsets and tool lengths correctly. Maybe I'll go single step at the beginning of the first run through of a profile to make sure I set the tool radius register correctly, then proceed. This is all to say that I use caution wherever a man is being relied on to make a machine setting, because that is where the screw-ups occur. My program will be okay in itself. Watch and learn from the first run of the program at the machine, make adjustments for feed rate, spindle speed, tool step-over and depth of cut in CAM, simulate, repost and go again.

OneCNC creates a template for every tool used. This is basically a small history of your settings used in a particular machining op. It is up to you whether you want to lock and save it, or, simply let it 'float' and absorb the latest settings that you used for that exact tool. If you machine families of parts, templates can really save a lot of clicking to create new operations that are similar to ones you have used already.

Templates work in all machining strategies, 3d, as well as stuff you could program from just a line drawing. Drilling is handled by a special 'wizard' that attempts to sort out the holes by size (if a model is on screen) or simply from points or circles if you are working 2d. Hole making operations can be saved as distinct patterns within the hole wizard, then re-applied to a brand new model that is put on screen. You still have to do the selecting of which holes get what, and so on, it is not full automation, but then, what two parts have holes that are identical. Most of the time somebody has to go through and make sure things are being properly drilled, if for no other reason than CAD drawn/modelled holes seldom show a conical bottom at a specific drill point angle, if the hole is blind.

I do such a wide variety of parts that I don't make that much use of (historical) hole making combination ops (using 3 or 4 tools) because I'd end up with a list so long I'd get lost looking for what was correct. I find it nearly as fast to just make new drilling ops on the fly, but that is not the software's problem, it's my circumstances.

Don't know if all those words convince you of anything, that's not really my intent, rather just relating how work typically goes for me. Other people could probably relate how much OneCNC sucks compared to what they went to afterwards. Me, I'm happy with what I've got to use. Sorry your Bobcad isn't working out for you, but that is why I left it behind as well, it was too much living in anticipation of the promised land

wheelieking71 said:

13engines,
I use FeatureCAM. FeatureCAM has a function called "automatic feature recognition" (AFR).
This is supposed to basically program the part for you (as you kind of vaguely described).
I gave up on AFR years ago.
In a great attempt to get this AFR to function in such a way that the software would create a logical machining strategy, and spit out sensible code.
I spent considerable time on my machine/tool defaults and attributes. This was not time wasted, because it helps immensely whether using AFR or not.
And, I still find myself tweaking attributes quite often.

Click to expand...

Veering a little off topic here, but AFR isn't the only method of feature recognition in FC. While I agree that AFR is absolutely useless, New Feature > Extract with FeatureRECOGNITION works well and I use it constantly.
FC is also capable of generating finely tuned paths, but I agree that there is way too much messing around and often-times pure guesswork involved in getting it to do so.

I have been determined to move away from FC for a while now, purely because of the bugs and instability, but there a few things holding me back i.e. the amount of work I've put into the tool library and posts, the fact that I know the post language like the back of my hand, the speed of making a functional (if not optimal) program etc.

gregormarwick said:

FC is also capable of generating finely tuned paths, but I agree that there is way too much messing around and often-times pure guesswork involved in getting it to do so.

Click to expand...

Agreed 100%. Manipulating 3-D strategies and tool-path in FeatureCAM is simply a pain in the ass.
2.5-D is actually pretty straightforward. I have very few issues there.
But, once you start surfacing, it is a completely different experience.
The simple stuff isn't too bad once you get some seat-time under your belt. But, more complex stuff will make you want to shoot your monitor.
And, some of the nomenclature they use is freakin' out there.

gregormarwick said:

I have been determined to move away from FC for a while now, purely because of the bugs and instability, but there a few things holding me back i.e. the amount of work I've put into the tool library and posts, the fact that I know the post language like the back of my hand, the speed of making a functional (if not optimal) program etc.

Click to expand...

I also am tired of the bugs! And bringing them to supports attention is a waste of time.
They treat me like I am crazy, and tell me the things that are happening are not possible.
And, the tool crib is freaking stupid. Plain and simple.

But, like you said, it is very fast. Print/solid to part is lightning quick compared to MasterCAM (the only other software I have experience with)
And, geometry creation in FeatureCAM is so good! I know, who "draws" parts anymore? LOL
Well, with no modeling or CAD experience, I do! And "drawing" in FeatureCAM is worlds better than MasterCAM.

I am locked in to FeatureCAM now simply because of how much $$$ I have invested, and I need a return on that.
It is fast, and that is important to me.
I have thousands of legacy files, hundreds of which are still very relevant.
And I do not have the time to learn anything new. But, I sure want to!

Fusion is very tempting. But, I hate everything about the cloud.

13engines said:

First thanks to all those that responded. I'm getting it that people really do use the 3D cam capabilities of their software. I also realize that I'm not going anywhere new until I get off this XP Pro operating system. Time for Windows 7 at least.

I should clarify that most of the parts I do have features that can be created with some form of standard tooling or a creative tool path. Many in vises or multiple twin vises. Many on fixtures I have to build. Once in awhile I'll get something that has curves that can only be created by some step over machining technique. My work ranges from fairly complex with 20-25 separate tools down to quick and easy and under 10 tools. Quantities from one or two up to 200. Most in the 25-75 range.

I ask to clarify a couple things. So my fellow programmers are selecting entire 3D models, selecting a roughing and finishing strategy, and in a minute you've got your program? How does one end up with 20 some tools? Or do you select each surface features and plow through each one while telling the software what tool and what step over to take and all that? I mean, after programming a complex part with many features and various chamfers, are you left with this large library of selected rouging and finishing strategies selected through your software, that together represent multiple tools creating multiple part features? What about drilling cycles? And do you as one person said, have to over time, develop very deep tool archives, so when you call up a tool, much of its values are already filled in? I'm still a tad lost as to what is actually accomplished in a nearly hands-off-and-let-the-software-do-it approach to programming.

The bit I wrote about first run gitters is because with my versions of BobCad, the resolution and quality of back plotting them over a solid model is practically useless. You can't see anything for sure.

I agree with what one person said in that trying other software will most likely expand my programming skills. That I can see. I'm looking to feel more competitive in the market, and I can imagine high end software could help me get there. As an aside, I've also nearly completed a ground up rebuild of a Mori Seiki SV-50 VMC with a pallet changer. All new screws and rails, bearings, you name it. It's a triple jump from where I am now in its speed and capabilities, both in hardware and control features, so I'm anxious to consider amping up my programming to take advantage of it. Also I'm nearly finished implementing a full 4th axis on both machines. Another unknown programming landscape for me to get hip on. Plus this new machine has probing and Macro B. I feel my plate getting very full in the programming department.

Again thanks everyone for taking time to respond. Highly appreciated.

David

Click to expand...

David,

Where are you at in Minnesota? I'm in the north metro.

The examples you see of complex models and one or two clicks to done are totally set up that way, pre-determined how they'd do it, they apply some templates, boom its done. What they don't show you is the tens to hundreds of hours put into those templates to make them work. For your general machining, yes you still select edges, faces, step-overs, and tell it what to do like you'd expect. Hands off programming really doesn't work that great for a small job shop unless you're creative enough to set it up properly, even then you'd probably want to set things up your way for specific parts.

There are some high end roughing and finishing strategies that work really well and will quickly produce toolpath, you still have to determine what all is necessary to get there, and if its all you need. Some of the finishing strategies are really quick and easy to apply, some not so much. It all depends on the geometry and knowing what your software is capable of.

Definitely get yourself out of 1998 and get a new computer with Windows 7(not Windows 10), proper graphics card, CPU, SSD HDD, and it'll make your life much easier.

wheelieking71 said:

Agreed 100%. Manipulating 3-D strategies and tool-path in FeatureCAM is simply a pain in the ass.
2.5-D is actually pretty straightforward. I have very few issues there.
But, once you start surfacing, it is a completely different experience.
The simple stuff isn't too bad once you get some seat-time under your belt. But, more complex stuff will make you want to shoot your monitor.
And, some of the nomenclature they use is freakin' out there.



I also am tired of the bugs! And bringing them to supports attention is a waste of time.
They treat me like I am crazy, and tell me the things that are happening are not possible.
And, the tool crib is freaking stupid. Plain and simple.

But, like you said, it is very fast. Print/solid to part is lightning quick compared to MasterCAM (the only other software I have experience with)
And, geometry creation in FeatureCAM is so good! I know, who "draws" parts anymore? LOL
Well, with no modeling or CAD experience, I do! And "drawing" in FeatureCAM is worlds better than MasterCAM.

I am locked in to FeatureCAM now simply because of how much $$$ I have invested, and I need a return on that.
It is fast, and that is important to me.
I have thousands of legacy files, hundreds of which are still very relevant.
And I do not have the time to learn anything new. But, I sure want to!

Fusion is very tempting. But, I hate everything about the cloud.

Click to expand...

It sounds like their AFR is the same as Mastercam's FBM (feature based machining). I have tried it a couple times (FBM) and I can't get anything decent out of it. I'm sure it works if you spend lots of time up front, but I think you would need different parameters for different parts maybe. I might be wrong, but if that is the case I can just save templates that have tools, doc, feed, stock to leave, and all that stuff if I wanted to make families of parts so what is the point using FBM?

I'm curious, what don't you like about drawing in Mastercam? I find it about as easy as anything else I've used, and probably the easiest since I have been with it so long. Couple things that may help -

Do you know that an entity (line, arc, etc) is "live" (it will be a light blue color by default if it is live) until you clock another command? So you can click the line icon, draw it anywhere you like, then you can go into the boxes at top of screen and change the length, angle, start point, end point. Also I have found quite a few people don't know this one, if you click line (arc) you can just start typing for a start point? So after you click the line icon or goto create>line>endpoint, a window pops up and asks for a start point, at which time you can type in coordinates (X,Y,Z if you don't specify a Z it goes to zero I believe), OR you can click in the graphics window. Same thing for endpoint, can either type it in or click in graphics.

Just a couple examples using a simple line, most of the 2d geometry responds the same way.

Mike1974 said:

I'm curious, what don't you like about drawing in Mastercam? I find it about as easy as anything else I've used, and probably the easiest since I have been with it so long.

Click to expand...

It's not that I don't like drawing in MasterCAM. It's just that FeatureCAM is worlds better.
You would just have to give it a try.
I hated FeatureCAM at first, because it was being shoved down my throat by a brand-new employer (who was a raging ass-hole).
That lasted about a week. I quickly realized how good it was after I started getting used to the work-flow.

Hey JFettig,

I'm over in Saint Paul on Pierce Butler Route.

Many have given me plenty to chew on. What you have said really coincides with my thoughts on the matter. I could never buy into the idea of a few clicks and you're on the floor making parts. Though I do bet there are some great roughing strategies. I'd also like to do more in HSM tool paths. I've done a couple manually for kicks and it's pretty cool. A little rough on the machine but...

Not sure ultimately where I'll end up, but I am looking to buy a computer with Windows 7, and I did buy Fusion 360 a couple days ago because it was selling on Amazon for 25 bucks a year. I'm sure I'll try it, but again, not sure it's where I'll stop.

Anyway... look me up (ShrapNell Machine) and stop on by anytime. I practically live at the shop. Or better yet, invite me over and show me how it's done at your shop. I could use a few minutes of mentoring. Or like I said in the OP. Would like to see how the real world does it.

Awesome, thanks for the invite. I'll contact you sometime and swing down to chat. My machineshop is just a couple machines and me running them part time, I primarily do engineering work. Not much I can show off without breaking confidentiality.

HSM doesn't have to be rough on the machine, when its set up properly its not abusive at all. You'll find that the HSM strategies in Fusion are very dependent on the values the user enters, as far as I remember it doesn't compute any of these for you or at least give you a starting point. I run SolidCAM and it does a pretty good job of setting feeds and speeds and engagement based on material selection and cut depths (some user input variables that need to be right or conservative).

I wonder how many have taken advantage of training by the manufacturer (or qualified distributor) for their programming systems? I am amazed at the number of CNC - CAD CAM users who have never had any formal training ( and by formal I don't mean a 1/2 day expiation from the installation tech) on their CNC control / machine / software. I'm a big believer in the 3 - 5 day class type training. Youtube is another resource. On line tutorials also. We have had guys come in from other shops who have used Master cam (in our case) for years, but never had any formal training and are floored when shown some features they never knew existed.