Setting Rapid Feed and Maximum Cutting Feedrate when Z rapid is different than X & Y

My machine has a different rapid traverse rate on the Z axis than the X and Y. How do I accommodate this in BobCAD-CAM v27?
X is 250 IPM
Y is 250 IPM
Z is 150 IPM

All axis are original rated at 100 IPM cutting

This machine can run faster than this because I have retrofitted it with AC servos and Teco drives, but for now I just want to use BobCAD, and I set Mach3 to run at the original specs above

There is no breakdown per axis in BobCAD, just two settings of Rapid Feed and Maximum Cutting Feedrate

Not sure what I should so. If I make the rapid feed 150, then it will be moving Z correctly, but X and Y will be 40% slower than they are capable.

What to do?

Should I just set the rapid at 250? I assume Mach3 will just say no and run Z at 150 max anyway?

Hi Jevs, I'm a newbe with cnc and bc but I'le take a stab at the question. By no means take this as anything I just figured I'd see if I have learned anything.... top end rapid speeds generally set in mach3 engine tuning to accommodate your equipment and they don't have to match each axis..... cutting feed rate is determined by the material, cut depth and cutter with the ball park speed automatically calculated in bc when creating features and tool paths!!! Z is a different speed most the time... Hope I'm close ...Enjoy the weekend

Dave

Yeah, I am in the machine setup of BobCAD. It has nothing to do with the materials or feeds and speeds used during cutting other than I assume it sets the limits to top speeds within what your machine can do. I think it just sets the max parameters that BobCAD will try to use when it generates the rapid moves and cutting moves. You cannot set for each axis though. I set it at 250 IPM max rapids so it would not limit X and Y rapids. This is too fast for Z, but I believe mach will slow it to the max anyway and I doubt it will get any where near any of this for cutting speeds. Not sure there is anything else I can do since BobCAD has no independent axis parameters for these in the machine setup as far as I can see. My Z can actually move that fast and faster, but that is beyond what it could do when they spec'd it in 1978. I don't want to hurt it :)

Rapid moves (G0) don't have a feedrate, so I'm not sure what BobCAD is doing with them.

If BobCAD is exporting G0 for rapids, then Mach3 will handle the rapid feedrates.

I have no idea either. I just know I am setting up the software following the tutorials and in the machine setup "Machine Parameters" you have to enter Max # of tools, Max Spindle Speed, Rapid Feed, & Maximum Cutting Feedrate.

I am just getting into this, so I don't know all the G codes or how they are used.

On Edit,,
after dinking around a bunch,I have found the rapid feed is used to help the simulation come up with a total machine time on its clock.
So whatever your controller is set at,that would be what you would set this.
To the OP,,,pick a number you think is an average from the 3 different axis
Simulation Time Clocks are not usually highly accurate anyhow.

G code back plot like Preditor Editor level 2 is better for real machining times.

Yes, I am not sure how that helps? Z still has a slower rapid than X and Y. That is the main concern I had. Don't want to over speed Z, but don't want to slow down X and Y. If you only get one setting for all 3, I have to assume you pick the fastest.
However if as ger21 says all G00 code rapid moves have no actual setting for the speed when used and the machine decides, then I am not sure what it uses this for. Maybe it only uses the Rapid Feed setting for simulation?? So it shows you in the real speed you might expect your machine to move.
I would assume it uses the Max Feedrate so it knows the actual limit it can ask a tool to cut.

I would assume it uses the Max Feedrate so it knows the actual limit it can ask a tool to cut.



Yes.
Many machines are not capable of the crazy speeds and feeds that small carbide tools ideally run at.So yes,it keeps the speed and feed at a usable amount.

Quote:

---

Originally Posted by jevs

Yes, I am not sure how that helps? Z still has a slower rapid than X and Y. That is the main concern I had. Don't want to over speed Z, but don't want to slow down X and Y. If you only get one setting for all 3, I have to assume you pick the fastest.
However if as ger21 says all G00 code rapid moves have no actual setting for the speed when used and the machine decides, then I am not sure what it uses this for. Maybe it only uses the Rapid Feed setting for simulation?? So it shows you in the real speed you might expect your machine to move.
I would assume it uses the Max Feedrate so it knows the actual limit it can ask a tool to cut.

---

jevs

Follow what ger_21 is saying and then pause and think backwards :-

1) The maximum speed setting for the rapid moves are in BobCAD for the simulation timings and should be set the same as your maximum velocity setting under the Mach3 motor tuning , if not then the estimated run times will be quite a way out.If the X,Y and Z have different settings then the actual machining time will be a little out when compared to the BobCAD times but won`t be too far out. They will also stop BobCAD outputting feed rates that are higher than the machine settings.
The max feedrate is there as you have rightly surmised is to limit the feed rate any tool can run at, actual feed rates for individual tools can be set at the tool in the tool library.

2) ger_21 is correct, the actual speeds of the axis of your machine are controlled by Mach3 not BobCAD. A G0 command is just a command to the machine to run at the maximum setting at the machine, has no relation to a rapid setting in BobCAD, BobCAD does not output a rapid speed, ony a G0 command.

3) BobCAD only outputs the cutting speeds, plunge feeds etc that are generated either automatically (System feeds/speeds) from the information in the cutting conditions and tool libraries or from information that you enter manually either in the Tool area at the Feature or alternatively in the tool setup, you can set each tool to cut at a specific rpm and feed under each tool parameters.
If you aren`t able to spend the time setting up your materials and cutting conditions the you can create a couple of tools the same size say a 0.5 inch for Aluminium, one for Steel, one for Stainless etc and set feeds/speeds at the tool in the tool library, that way you will always have the correct speeds/feeds being output by BobCAD for your tooling/machine capabilities to suit the material :D

Hope that helps :D

Regards
Rob
:rainfro: :rainfro: :rainfro:

Rob,I just figured it out and edited above as you were posting :)

I know rapids only started being used in V26

Quote:

---

Originally Posted by jrmach

Rob,I just figured it out and edited above as you were posting :)

I know rapids only started being used in V26

---

Yes, V26 was when BC started with the generated setup sheets so rapids were needed for generation of the timings, as are the X,Y and Z distance limits :D

All good stuff :D

Regards
Rob
:rainfro: :rainfro: :rainfro:

All makes sense.
I did a bunch of reading about setting up tools and stuff. This looks like it is going to take awhile. I still am not sure how I will set all the tool heights and stuff. I do have a 7 tool changer. I also have an electronic touch off plate and a probe. I was thinking to use the touch off plate and just have it touch off each time it changes tools or something.......lot to figure out still. My tool rides in a turret on a bearing, so drawing the tools is going to be fun to figure out. I think I will have to draw the turret as part of the tool holder.

I may need to suggest BobCAD make setting up those speeds for each axis separate. I know there are many machines out there that have Z different like mine. I looked up specs on various machines just to see.

Quote:

---

Originally Posted by jevs

All makes sense.
I did a bunch of reading about setting up tools and stuff. This looks like it is going to take awhile. I still am not sure how I will set all the tool heights and stuff. I do have a 7 tool changer. I also have an electronic touch off plate and a probe. I was thinking to use the touch off plate and just have it touch off each time it changes tools or something.......lot to figure out still. My tool rides in a turret on a bearing, so drawing the tools is going to be fun to figure out. I think I will have to draw the turret as part of the tool holder.

I may need to suggest BobCAD make setting up those speeds for each axis separate. I know there are many machines out there that have Z different like mine. I looked up specs on various machines just to see.

---

No offence jevs but I`m not sure you have it 100% just yet :D :D It doesn`t matter at all what speeds are the BobCAD for rapids, your machine control handles all that, if the max speed for an axis in your Mach3 controller is 300 inches p/m then that is what you will get when the control recieves the G0 command in the code, even if it was set to 1000 inches p/m in BobCAD it will not go faster than the axis setting in Mach3.

So best to forget about that side of things, I stopped messing around with the simulations a long time ago, as long as it produces a reasonable guide of machine time per operation and an overall time then that`s all I need/worry about :D :D
You will have to spend a lot of time creating lots of solids for a machine simulation but unless you have paid extra for the full simulation is will be time wasted because you won`t have it working on screen as per your actual machine :(

If you have any spare time at all :D then it would definitely be better spent working on your tool library, materials library and your cutting conditions, they are way more important to the smooth day to day operation of your machine.

I have a touch off plate system on one of my mills, what I have done is write a few toolchange programs that cover any amount of tools I need for a specific job, I put all the tools in the carousel and set one tool as the Master Tool, then I just run the tool change program and it runs through all the tools and sets the heights in my Mach3 tool library, unless you really want the machine to check each tool at every toolchange which takes a fair amount of time then I would advise you do as I have :D :D :D

Definitely easier/quicker :D

Regards
Rob
:rainfro: :rainfro: :rainfro:

I do get it, it does nothing to the G code. Figured that out yesterday. I know it just uses it for time estimates, or simulations....However, if you want more accurate simulation and time estimates, you need different settings for each axis. I realize it does not affect how fast it moves on rapids :)

I do have the full simulation and also the predator editor which does a simulation. From what I saw, once you set up your tools for machining anyway, that the built in simulation just uses that info? I did not see where it was extra work to run the simulation as far as setup goes?

That sounds good on the tool changing. I still don't fully get that, but I am working on it. I figure I will make a new thread asking all my new silly questions.
I am not sure how to hook up my probe and my touch plate. I am wondering if they have to share an input and be connected in parallel, or if they can each be separate....trying to figure this out now.

Thanks.

Quote:

---

Originally Posted by jevs

I do get it, it does nothing to the G code. Figured that out yesterday. I know it just uses it for time estimates, or simulations....However, if you want more accurate simulation and time estimates, you need different settings for each axis. I realize it does not affect how fast it moves on rapids :)

---

OK, just checking :D Reason I and most others don`t bother about it is that the amount of time spent actually going up and down compared with back and forth is usually a very small amount but if you feel you need it then by all means send it in to BC for the developement team to look at :D :D

Regards
Rob
:rainfro: :rainfro: :rainfro:

I am sure I don't need it at this stage and maybe never. I just want to make a part here and there for myself for other projects, so the time it takes is not critical. I won't be paying myself by the hour unfortunately :(

I am going to post another thread. My head is spinning on setting up tools. I am starting some coffee, so maybe I will get focused soon. I feel like it is taking way too long just to getting to cut a part....

I need to make this...

Personally,I would quit worrying about your rapids.
There is a lot of software to learn here.
If you have Preditor Editor level 2 ,,, here you go ,,you think your mind is spinning now,take a look at this..

Yeah, I move past the rapids thing yesterday. It was a good exercise though, because I found I had them set too slow on the X & Y and too fast on the Z in mach. So it did some good....

So, what would you do next if you were me?
My machine is working with Mach3 fine.
My machine parameters and post are setup in BobCAD
I have not cut anything though.
I have nothing setup anything with tooling in software or actual tools. I am not sure what I have to do as far as measuring the tools in the tool holders and stuff?
My part is designed.
I do not have my touch probe or touch plate wired in (not sure how to have both those hooked up?)

So, what would you do next if you were me?

Spend a lot of time here https://www.youtube.com/user/Depoalo...view=0&sort=dd

Also the Mach forum should be of big help.I know nothing about Mach,so I hesitate on telling you how to set-up your offsets.
You do not need a tool probe and touch plate though.There again I hesitate giving you information on how I do it because my machine is Worlds different than yours,but there are other ways involving a piece of paper and an edge finder.That is how I do it.
Engine Guy is a whiz with Mach,maybe he can explain way to do it in Mach the way I just described.It will get you going faster,which is what you want,right?

Mach isn`t any different for tool setting, I use a slip guage (More accurate than jrmach piece of paper although that works fine as well).

Normal way I do it is I have a tool holder with a piece of ground bar in it (You can use any tool though) and touch it off on either the bed or the workpiece, doesn`t really matter which, that tool num ber is set to 0.00 for tool length in Mach and is set as your MASTER tool, after that all your tools can be touched off to the same point as the master and they will all be either longer or shorter when set in Mach, so in the tool library in Mach what you will see is the difference between each tool and the master, not the actual length of each tool.

Don`t worry about the tool lengths in BobCAD too much, it`s nice to have them accurate as you have a better simulation but they don`t affect your code in Mach, all you will get for tool height will be a line of code something like this :-

G43 H1 Z0.1

That would bring your Tool #1 to 0.1 inch above your job, the G43 tells Mach to go get a tool length and the H# tells it which one to go get.

For this to work right you will also need to have set up your workpiece offsets, particularly the Z one, again you can use your master tool to touch off in the X and Y for positioning although this will depend to some extent on what type of fixture/vise you are using.

When doing a shape like you have I would always draw it with the centre of the job at X and Y zero, that way it is very easy to machine the shape from your stock slightly deeper than the thickness of the part.
That can be done as an advanced pocket operation for both the outside shape and the inner shape.
Then after you have done the desired shape machine out some soft jaws in the vise and machine off the excess material from the back of the part, if you are going to run a small chamfer to the part for de-burr/cosmetics then that is why you would do the soft jaws, if you are finishing it off by hand de-burr then the machined soft jaws are not required.

I see you have some nice solids there for your part :D for a simple 2D job like your part there is no need for all that, a simple 2D outline is all that is needed to be able to generate the toolpaths.

If you need any help with getting the Features done and tool path generated quickly then Zip up your solid and upload to the thread here and someone will take a look at it for you :D :D

Regards
Rob
:rainfro: :rainfro: :rainfro: