Sprutcam and 4th axis

I just downloaded the demo version of the latest sprutcam software (5.4 something) and am curious about the 4th axis functions. The website shows that they can now do continous 4th axis machining although there doesn't appear to be any tutorials on these functions. I am trying to evaluate sprutcam versus visualmill for 3 and 4 axis machining. The biggest consideration for me with the fourth axis is continous 4th axis function otherwise I would do manual indexing and save the extra cost of the 4th axis machine. Can anyone give me an idea of the 4th axis functionality of sprut? I think the VM is a little easier to use, but sprut doesn't seem that bad, considering the learing curve, but the sprut price is attractive.
Thanks for yor feedback.

This thread http://www.cnczone.com/forums/showth...light=sprutcam has some info and videos as reference.

Try posting on the Sprut tech support forum:

http://forums.sprutcam.com/forums/

I've seen a tutorial running from Build 5.41 that seems to work fine but have yet to try it myself.

Mike

Why is it that there are so many videos of SprutCAM simulating coordinated 4th axis movement but no video of someone walking through the build process?

I've spent my entire weekend trying to get SprutCAM to do a simple 4th axis part, nothing complex just a simple (positional) example and it doesn't work. It never writes G0 A180 to gcode. I've even expressly added it via an Auxiliary Operation. It appears to do it correctly on screen but it doesn't generate any 4th axis code. I'm using Build 5.41 and using the PCNC1100 postprocessor, is there a newer post processor than this:

[SprutCAM postprocessor]
Version 4
NC Mach2
Machine PCNC1100
Date 08.06.2007
Authors J A Prentice
Comment Adapted JAP Rev 4A (June 2007)
Extension TAP

If you belong to Dave Pearson's tech support forum you can see a video tutorial on a 4th axis op and get a bit of email or Skype phone support.

Here's the web site:

http://www.download.sprut.co.uk/Supp...ex.php?act=idx

I have a few post processors for the Tormach from various sources and a couple of them are dated later than the the one you list, assuming that the 08.06.07 date format is European and means June 8, 2007.

At least one of them came from Yuri at SprutCAM and another may have come from Tormach. I can email you the one I've been using, but it is dated the same as yours. You could try one of the ones dated later but I really think you'd be better off checking with Yuri to see which one is most recent and make sure it isn't a "beta".

BTW, the latest build is 5.47 but I've read that it is bug fixes only with no new features. It would be good to get that confirmed by Yuri, though.

Mike

All -

I think I have finally broken the 4th axis code, but still have a few questions. I'll get to those later.

I have attached a zip file including two IGES files and a SprutCAM file. The first IGES file, SprutCAM_4th_Axis.igs, is the part for which you want to create a toolpath. The second file, 4th_Axis_Fixture.igs, crudely approximates the 4th axis rotary table, chuck, and whatever else you might want to avoid cutting. Both of them are already included in the SprutCAM file, SprutCAM_4th_Axis.stc. I wanted to make sure you could recreate my work if you wanted to try.

I'm using SprutCAM 2007 build 5.48, so your mileage may vary. Also, note that you will need the recent "MULTIGOTO" post in order to post a G-Code program using this method.

Here are the steps I took (as I recall) to create the toolpath. Please don't shoot me if I forgot a step. You can always pay Dave to help you if you get lost...

1. On the 3D Model tab, Import the part file.
2. Select all of the surfaces of the part (Ctrl-A will do it).
3. Right Click on any of the selected parts. You will see a popup menu.
4. Select 3D Model | Properties, and a popup window titled "Objects Properties" will appear.
5. Select the Machining tab.
6. Uncheck the Double Sided checkbox and then click OK.
7. Select all of the surfaces again if they are not selected.
8. Right Click again on any of the selected parts.
9. This time, select 3D Model | Inverse from the popup menu.
10. Now click on the Machining tab.
11. Select the Machine line and click on the Parameters button.
12. On the popup that appears, click on the Machines tab.
13. Select 4-axis milling machine (A) and click OK.
14. On the end of the menu bar of the program, click on the icon for create coordinate system. It should be the little white rectangle next to the box that says, "Global Mill CS." A popup window will appear entitled, "Definition of new coordinate system (CS)."
15. Click on the Rotary Axis tab.
16. Click in the Position box and type 360. Click OK.
17. Define the workpiece. I simply used a cylinder around the part, along the X axis.
18. Select Machining and click on the New button.
19. Select Tool-End 5D Machining from the Finishing tab. Click OK.
20. Click on the Parameters button.
21. Select the tool. SprutCAM seems to have a bug in that it will only use the center point of the tool to compute Z height in this mode, so you should probably plan on using a Ball Mill. Enter your favorite feed and speed.
22. On the Strategy tab, select Axis Z Position as the Safe Axis, and set the level to something larger than the largest radius of the part. In the case of the example, I used 1.1 inches.
23. At the bottom of the Strategy tab, play with the top and bottom levels until the toolpath is what you want. In this case, I used 0.5 and 0 inches.
24. Also on the Strategy tab, in the Machine State box, select Workpiece Coordinate System and pull down RotAxis 360;0 (the local coordinate system you made in steps 14 through 16).
25. Change Local Coordinate System to RotAxis 360;0 in a similar fashion.
26. Click OK on the Parameters window.
27. Under the Machining tree, click the little plus marks until you see Job Assignment. Select Job Assignment.
28. Add the faces you would like to machine using the Add Drive Faces button.
29. SprutCAM makes a group of the faces you chose. In the box below the Add Drive Faces button, select the group (Group 4 in this example). Click on the Properties button that is on the same line as the Add Drive Faces button. An Item Properties popup will appear.
30. Select the Alternate front side checkbox.
31. Change the step method to Distance (or whatever you want). Change the Step amount to 0.05 (or whatever you want; it defaults to one step).
32. Click OK.
33. Now click the Run button and let SprutCAM create the toolpath.
34. Simulate and enjoy.

The questions: As I mentioned in Step 21, I think SprutCAM has a bug in this mode in that it will only work correctly if you choose a ball mill. Every other tool I tried will crash on the cone shaped portion. I found this before when I tried to get a 4th axis toolpath, and here it is again. You can change to using the side of the mill by choosing Flank on the Strategy tab, which may give a better finish. That may be a way to get a flat but sloped surface (but no sharp corners).

Also, this part is pretty simple. Have any of you tried anything more exotic, like an eccentric cone? Dave's example of a camshaft is eccentric, but also simple in that it only has flat (horizontal) areas to mill. I suspect SprutCAM will fall on its face with a more difficult part.

Try this out and let me know how it goes. Maybe we can resolve the questions by just tinkering with the parameters.

Regards,

- Just Gary

P.S. Well, I tried to attach a zip file. It is way under the max size allowed, but failed to upload several times. Any ideas?

I am just getting started and learning my new PCNC but my goal is to do true 4 axis machining.

I would really appreciate if you could email me the "zip" file you were trying to upload here.

my address is "[email protected]"

Thanks in advance!

Quote:

---

[SprutCAM postprocessor]
Version 4
NC Mach2
Machine PCNC1100
Date 08.06.2007
Authors J A Prentice
Comment Adapted JAP Rev 4A (June 2007)
Extension TAP

---

Looks like you need to download the current postprocessor from the Tormach site.
The other thing I think most of us need to remember is that most more expensive software comes with training and or is available for purchase. One way or another you will have to pay to be trained. If you want to try on your own I say go for it, but if there's help go for it, after all I didn't spend $18,000 to beat my head against the vise wondering how to. Like I said before 1 months training broke the ice for me as well as downloading the SprutCam manual and having Staples print it off for me double sided pages and bound-$20.00 well worth it also. $60.00 well spent.
Also people who want to post info is great, and I thank them too. I also think most 4th axis owners have machining background and are familiar with another CAM software. I have my Journeyman Machinist card but had no prior 4th axis machining of anything more than running a conversational mill. The tutorials helped I could do them when I wanted and not wait for someone to post a response.
Gary, keep up the good work.

Grrrrr. I'm having troubles with posting messages to this site.

Let's try again to post the ZIP file without the SprutCAM file. At least then you'll have the two IGES part files and can attempt to recreate my work.

By the way, I have crammed several of the sprut.ru web pages through Babel Fish to try to get a few tips. The site is full of marketing hype, but not much else. The best thing I learned is that "sprut" apparently means "octopus." I don't really speak russian (although it is phonetic, and their technical words sound a lot like ours), so I don't know if Babel Fish got it right or not. I tend to agree with it.

I really do like the software, but that doesn't mean that I don't have tentacle marks...

Regards,

- Just Gary

Gary,

I have web space and am happy to host it for you and post a link. If you like, email it to me at djborden (at) gmail.com

David

Thanks Gary,

Here you go guys: www.gtmbuild.com/misc/SprutCAM_4th_Axis.zip

Right click and "save target as" to download.

David

justgary,

I received your "iges" files and followed through your step-by-step instructions. My first question to is "HOW ON EARTH DID YOU FIGURE ALL OF THAT OUT????"

The simulation seemed to work where the rotary axis rotated a full 360 degrees for each profile increment. The only thing I noticed was that the rotary axis was not operating synchronized with the linear axes. I'm sure that wasn't the objective with your trial but I wonder 'how' and 'if' that can be done.

Also, when I posted the code, there were no rotary axis moves in the file. I think you mentioned that you had that same problem but found the fix. Can you tell me how you did it?

saabaero -

I put on my data mining helmet, clicked on the headlamp, and went prospecting out on the vast internet. I found just enough nuggets of information to piece together the motivation to keep trying. Sometimes all I had to go on was the trust that it could be done. Lucky for me the batteries in the headlamp didn't die while I was still mining!

SprutCAM made it pretty easy to tell when I had done something wrong, because I got it to lock up or instantly crash several times. I have learned over the years that once a crash is repeatable, you probably should try something else.

If you are talking about synchronized A axis as in helical milling, I have not tried that. It would not be too hard to code a helix by hand, though, since all of the axes run at constant rates, even on a tapered one. Sometimes you just have to take the bull by the horns and hand code to get what you want.

I'm confident that SprutCAM will eventually do it easily and correctly, but for now I'm glad it does at least some of it. Tool-end milling, as the program calls it, is just that: they simply rub the end of the tool all over the outside (or inside, if you skip a step) of your surface while they incrementally turn the A axis. Automatic toolpath generation is quite a trick in three axes, and I imagine that four or five axes just makes it exponentially harder to do. And then you'll probably want it somewhat optimized...

Right now I'm working on a 4th axis toolpath for a twelve-sided pyramid that tapers to an eccentric cylinder. Rather than try to explain it, I'll attach a picture. So far I'm not satisfied with the toolpath or the run time. I'm redrawing my part now that I know how SprutCAM works, and I'll draw what it needs to see so that it will cut what I want. It's not too hard to adjust lengths and slopes to account for the cutter since SprutCAM won't do it yet.

As for your last question, go get the latest postprocessor file. If you have the Tormach-only version, it is this file, or if you have the open version it is this one. As mentioned several times before, the new postprocessor file has the MULTIGOTO command capability, which SprutCAM uses to drive all four axes at the same time.

Regards,

- Just Gary

justgary,

You certainly did some fine detective (mining) work in developing that procedure.

I thought that I had the latest post processor but I'll have to double check.

What I had in mind was 4 axis synchronized motion as in doing a turbine impeller blade or something that required varying "Z" height while the 4th axis was rotating.

In looking at the recent model you posted I'm thinking that may need synchronized "Z" and "A" axis motion!?

saabaero -

I have played with the part that I posted a picture of a few days ago. I now have a toolpath that I am satisfied with, although I have not yet tried to cut it. The best part is that I'm getting much more comfortable with the small details in SprutCAM, and I can get what I want a whole lot quicker than before.

The bottom line is that you have to play with the settings in SprutCAM, but it will definitely give you a coordinated X-Y-Z-A path. In simulating the part I have, I can clearly see all four axes working together in a coordinated fashion to put the flats where they belong. It's actually impressive to watch.

I did have a glitch in one path that I had to fix by hand, and could not get SprutCAM to correct it. I fixed it on the simulator page by editing the offending lines before posting the G-Code. You can do that as long as you don't rerun the toolpath (which would clobber the fix). I think I'll also remove a lot of the air cutting that I see before I cut the actual part. Right now the job is looking like it will take 100 minutes to cut, but I expect I can cut that in half or better by removing needless motion.

I think that as long as your tool will reach all parts of your turbine blade without crashing on another part of the blade, you should be able to get a useful toolpath out of SprutCAM. It might take a while to cut, but it should work.

If you have an IGES file of your blade, send it to me and I'll take a look to see what I would recommend. Also tell me what types of tools you have in case I get a toolpath for part of it. I might as well use the tools that you already have...

Regards,

- Just Gary

I'd be really interested in seeing the simulation for your part. You can email the file to my yahoo address that you sent the other file to if you have time and don't mind.

I think you have the right idea in attacking such complicated problems in that you have so many more opportunities to learn all sorts of other things in the process and afterward the difficulty of other projects pale in comparison.

I was trying to think of an example of a part that would require 4 axis synchronized motion when I suggested the turbine example.I don't actually have an application for one at the moment (but you never know). The only problem is that in order to articulate the cutter between the fins or the turbine wheel I suspect that 5 axes may be necessary.

Actually, one very real application I do have for true 4 axis motion is in fluting rifle barrels. I have done straight flutes on tapered barrels but would like to do spiral flutes on tapered barrels.

I am in the process of installing and wiring the additional stepper drive and have a two different size rotary tables that I need to fabricate mounting brackets for before I can actually have 4 functional axes. However in the meantime, I really want to understand Sprutcam's abilities and limitations as much as I can.

I really appreciate you sharing your experiences with the group. With so little documentation available for the Sprutcam it really helps if we can learn from one another.

I'll see what I can do about creating a video of the simulation.

I took about ten minutes yesterday and drew the attached "turbine" just to see what SprutCAM would do. Please note that I just threw it together, and it is not supposed to represent any working turbine design.

I then took another ten minutes in SprutCAM to see what it would do, and in the immortal words of Scotty, "what came through, didn't live long." Maybe I'll give it another stab sometime just for the experience.

To flute a tapered rifle barrel, you only need to move X, Z, and A. Also, they all move at constant rates. In other words, you don't even need a program to do it. Suppose your flute starts at X0 Y0 Z0 A0 (and for this discussion, the zero Z value is already plunged into the work). Now suppose that the flute should curl 15 degrees and run 12" in X and -0.5" in Z to account for the taper. Further suppose that you had already set your speed and feed to your favorite numbers and started the spindle. The MDI command G1 X12 Z-0.5 A15 will do it.

Of course, you'll probably want to do it in Z steps, but if you write them on paper (or even in a text editor so you make a program that you just load and run), you can easily keep track of them. Rotate A to the new starting point and zero A, then run it again for the next flute.

Regards,

- Just Gary

Hey, you may have just come with a new design for an advanced jet engine turbine wheel!

As far as the rifle barrel fluting is concerned... Wow, I never even thought of that. I always amaze myself at how complicated I can make the simplest problem. Your solution certainly saves a lot of steps in having to create a CAD model, import it into Sprutcam and generate the tool paths.

I always say that anyone can come up with a complicated solution to a simple problem but it takes a genius to come up with a simple solution to a complicated problem.

saabaero -

I over complicate things all the time. It's probably a function of having cool toys to use. Of course, a year later it dawns on you that you could have just tightened the screw instead of making a thicker replacement part. Oh, well, it's fun to think up solutions to problems.

Post a picture of your fluting job when you get done!

- Just Gary