Sprutcam and 4th axis

[RP Designs]

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.

[DareBee]

This thread Looking for cad/cam software to use on Hobby X2? has some info and videos as reference.

[MichaelHenry]

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

[Cairns]

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

[MichaelHenry]

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

[justgary]

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?

[saabaero]

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 "x1y2z3usa@yahoo.com"

Thanks in advance!

[R.DesJardin]

[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.

[justgary]

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

[David Bord]

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

[David Bord]

Thanks Gary,

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

Right click and "save target as" to download.

David

[saabaero]

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?