Software for rotary axis

[ejsp]

I wish to put a rotary axis on my shopbot.
I have not seen any good software to permit control of a rotary axis.

Any one know of such software?

[br928]

NO....good luck....search the forum under "indexer"

[myxpykalix]

I'm not aware of anything that SB has other than the indexer control within the Control software. Bill made a "Rope Twister" wizard that might help you. I'm sure it is posted somewhere.

[Gary Campbell]

Edward...
Are you looking for CONTROL software or DESIGN software?

ShopBot Control software 3.xx will control a rotary 4th axis. From reading posts concerning indexers, I assume ArtCAM Pro works for design, but will let those who actually have the indexer to confirm.
Gary

[scottcox]

Edward,

Shopbot indexer files can be created in a number of different ways.

1. You can create your own M5 commands using Windows notepad. There's at least one example on the Shopbot Wiki.

2, You can use Artcam or Cut3d (or Rhino and Deskproto so I hear).

3. You can convert any XYZ file into XBZ. B=Rotary Indexer in degrees. A simple conversion from max Y in inches to 360 degrees.

...and it's handy in other ways as well for sanding in the round and workholding for many shapes.

.... but that said, I'm sure there are many other ways to use the indexer.

Any other ideas, folks? How else do you use your indexers?

Scott

[blackhawk]

I do mechanical design work for my "real" job. I can create a 3D model of say...a table leg with no problem. Will Cut3D/Partworks be able to turn this into a cut file for use with an indexer? I don't have Cut3D/Parworks yet, but wondered how the software would know if you had an indexer in use. Does the software have an option to select rotary cutting before it generates the cut file?

[scottcox]

Brad,

Cut3D would give you 4 raster toolpaths for top, bottom and sides. You can even modify it to include 4 more toolpaths rotated 45 degrees to the first set. The indexer would basically be used only as a work-holder turning it a specified number of degrees between toolpaths.

ArtCam "unwraps" your model and writes an indexer file, rastering along the indexer axis, slight turn of the indexer then rastering back, etc.. I believe that Rhino and Deskproto do something similar.

Keep in mind that you can use "flat" toolpaths anywhere on the indexer-held piece. A mortise on a table leg would be a good example. A v-carve file for a flat part of the table leg is another.

You can also insert rotation commands into a string of "flat" files if you design it for such.

I would love to hear some more.

[blackhawk]

Scott - I believe that I follow you. Your descripition would be for a 4 sided square table leg with carvings on each face. What about a traditional table leg that is square at the top portion then has turnings all the way to the bottom? Would Cut 3D know to continuously turn the indexer at a certain RPM as the X and Z do their thing along the round portions?

I guess in that situation you probably wouldn't even need an indexer connected to the machine. Could you just throw up a regular lathe bed on the shopbot and just turn it at a constant RPM? Then use a 2D cut path with the y axis flipped to a Z axis and move real slow. But then how would you handle a deep profile? You would need some type of roughing operation or you would probably snap your cutter.

[jim_stadtlander]

Brad, I am currently delving into all the aspects of this also. What I seem to have found out so far is that Cut 3D will not create a toolpath that turns the piece while cutting(please, anyone, correct me if I am wrong!!!!). Shopbot has software included that does turning of a profile like you mentioned in the second paragraph. What design software are you using for 3d objects? To my knowledge, Artcam cannot truely think in 4 sided objects.

Some problems that I have incured and maybe someone knows of a fix? Cut 3d cuts side one, turns cuts side two,turns, etc. Thus, It spends time cutting areas that have already been machined, making for long cutting times. Makes sense to you?

With regards to your second paragraph and cutting deep profiles. Yes, the Shopbot software(included) can do it by means of a profile, BUT it takes several passes to work your way in to deeper areas and it goes over the entire profile while doing this, thus taking time to go over the shallow areas(following that profile) and not cutting anything there, resulting in long cutting times. It doesn't know how to figure out a roughing pass, like in flat sides.

Scott(or anyone)- Where does a model come from that Artcam needs to "unwrap"? And how does it make an Indexer file? I can only "trick it" to think it is an indexer file.

Hope any of this helps, and maybe someone out there can answere the problems to which I have I have mentioned to help you out too...Jim

[rnels]

Jim,
You can create a relief in ArtCam and do a Z level rough and then a finish pass on the indexer. You could set up your model to the width you need and the height would be the circumference you wanted (diameter * pi(3.14...). Then do a 2 rail sweep with a profile shape and the rails at the ends of your model. Then create the rough and finish passes for this relief. When saving your toolpath ArtCam has a postprocessor for the Shopbot indexer X and Y axis (have not tried this though).

You can get 3D models and unwrap them into ArtCam then toolpath them from there. I have not had time to experiment with this much yet.

The thing about the profile is you don't need 3D capability you can create shapes just using the profile vector (the hard part for me is creating the relief model in ArtCam). It takes time to do the Z level rough and finish also.

Randy

[waynelocke]

I have not had a chance to try this but have been thinking about it for a while. You should be able to do what Randy describes by making a file in Partworks 3d and making the "y" material size the circumference of the part.

You should be able to then use the VI command to make the Indexer the Y axis instead of the B. With the right unit values it should cut on the indexer like a regular flat file. The shopbot should do the conversion automatically.

Not as elegant as Artcam but I think it should work

[khaos]

I'm pretty sure this is the method Brady talks about. Just set your VI values so the 'end' of the works butts against the 'begining'

Although he is talking about an indexer her you can get the idea and use it for cutting.

http://www.talkshopbot.com/forum/messages/312/29601.html

[waynelocke]

Yes, that's the general idea, although Brady's use of the probe on the indexer is a little different since the file would begin as wrapped model, i.e one revolution would be probed as 360.

If you wanted to wrap a file around a cylinder which was say 12" in circumference you would make a file 12" wide. The normal indexer values making one revolution in 360 would not work and it would seem that you would have to divide the unit values by 30 to have it correctly machine.

I think that you would a different unit value for any given circumference. If you used the normal setting the control software would not discern the difference between a 12" or a 30" circumference. You would also have to zero to the finished diameter of the surface.

Having said that, math is not my forte and stand ready to be corrected.

[jim_stadtlander]

Hmmmm...... In response to the VI commands, I posted a question/problem a few post earlier to this. Now that problem could be because I am not able to get the postproccessor figured out yet to do a rotary file??? Please check out my earlier post to what happens when I swap the Y for the B axis.

I do not see a postprocessor for a shopbot indexer. I see a few listed separately under "rotary" but doesn't give me shopbot file.

As far as software goes, is there any that can cut one "side" at it's edge and then across that surface(going to each side of the center-line) turn it so many degrees and still keep track of the areas that it has cut and still needs to cut?

Edward and Brad, hope some of my questions are helping you out too......Jim

[Brady Watson]

The indexer can be used in many ways. 1st, it can be used simply as a table rotation device, where the workpiece is cut using X,Y,Z coordinates while remaining completely stationary until the operator gives a table turn command. A practical use for this would be to set your material between centers, zero to the top of the block and cut the 1st side of a 4-sided 3D file toolpathed in Cut3D/PartWorks3D. When the 1st side is complete, give the command to rotate the table/indexer 90° by doing a MB,90 - then cut your 2nd side. No need to zero out the B axis since a 3-axis post never writes code for it. (But you will need to level & zero the B before you cut anything initially)

The Indexer can also be used as a Rotary Axis in TWO ways:

1) Code from your CAM software with Rotary post outputs code with B moves in it. This converts circumference distance in inches to DEGREES. The indexer moves IN DEGREES as it rasters back and forth cutting out your 3D part.

2) Code from your CAM software is outputted from your 3D program Just as your normally would output a 3D file for XYZ cutting and you TRICK SB3 into thinking that the Indexer is an X or Y axis, after locking your REAL X OR Y axis down to keep it from moving. (clamps etc are a wise idea) The 3D part needs to be unwrapped so that it is flat when you bring it into toolpathing software. Careful planning BEFORE you scan a part, will pay in spades later. If you scan with the SB probe on the Indexer and trick it into thinking it is just a flat panel (tell it the indexer is Y axis, for instance), then you can bring that file into CAM, toolpath it like any other 3D file and TRICK THE INDEXER in SB3 and cut the part out on the indexer. As others have pointed out, you need to know the circumference of the part and convert that into inches (read what Wayne wrote above)

Creating files for rotary cutting & hacking existing full 3D files is a whole other topic...

-B

[rnels]

Here are the two post processors I got from Brady for ArtCam Pro. I have not tried them so no guarantees they work. They would go in the program files - Artcam pro ver under postp.


Shopbot indexer x
Shopbot_IndexerX.CON (http://www.talkshopbot.com/forum/messages/312/Shopbot_IndexerX-31221.txt) (1.5 k)


Shopbot indexer y
Shopbot_IndexerY.CON (http://www.talkshopbot.com/forum/messages/312/Shopbot_IndexerY-31222.txt) (1.4 k)

Wayne, I don't know the math so well but I noticed on my own software when testing with logs and using degrees the turning seemed to complete at the same point with a difference of 1 inch in diameter in the log (in other words I used a log blank of 6 inches for one and a log blank of 5 inches for another and used the same .sbp indexer file and they turned out the looking pretty much the same except one was larger in diameter and the detail was spread out more). In my program I convert the whole .sbp file using the maximum Y value being 360 degrees so I believe the one revolution in 360 degrees would work (and has worked in my testing however I only have tested up to 6 inches in diameter or approximately 18 inches in circumference). In my testing I have not had to change the control software settings between sizes. I use the default 13.8889 unit value for B on my prtalpha.

Jim, not sure exactly what you mean but if that's what you have layed out in your PW or ArtCam model then the toolpath should be the same for a flat file as a rotary file as far as keeping track of areas to be cut etc.

Randy

[blackhawk]

You guys are losing me a little bit, but let me run this by you guys. I based this idea on how to make a short table leg from Brady's #2 option above. I am thinking in terms of using Cut3D from Vectric. (I don't see me affording Artcam Pro for a very long time). I don't have Cut3D, but am planning on purchasing soon. The first picture is done in my CAD software as just an extrusion (unwrapped) table leg. The leg length is 12", and the unwrapped length is 9.425". 3" is largest diameter, so 3" x pi = 9.425" for circumference. I made the the thickness as 1.5" at the flats (3" dia/2). If I sent this file to Cut3D as an STL file, then made the indexer be the y-axis, then set the unit values to 38.2 (360/9.425), would the part turn out as shown in my 2nd picture? Where do you input the unit values?

6664


6665

[rnels]

Brad,

I have a dedicated 4th axis for the indexer so I don't have to trick SB3 so I'm not familiar with that issue. It looks like the file should cut as you expect but I'm not sure about the unit values. Believe VU will get you to the spot for entering unit values.

Randy

[Brady Watson]

What gear ratio is your indexer, Brad? Alpha/Standard?

-B

[blackhawk]

Brady - I have a PRT alpha machine with the 7.2 motors on the X and Y. I currently don't have an indexer. I am just feeling out how the indexer can be used before I buy one. I planned on buying the indexer from Shopbot. Their pricelist only lists an indexer for a PRS alpha. Would it work with a PRT alpha?

Has anyone tried using an STL file in Cut3D from a 3rd party CAD program?

[jim_stadtlander]

Would it be better for Brad to just use the Indexer program under "tools" in SB3 ? Will Cut3D take longer/shorter to cut this than using SB3?

Brad, I certainly will try cutting it for you if you email me the File/model. I have as much to learn as you!! I am thinking your math has to go one step further, at least if I follow Wayne's logic above. So.....360 divided by 9.425(circum.) = 38.2, then UV divided by 38.2 = FINAL # ---Is this right, for those who would know?

Randy, Thanks for those post proccesors. Can't wait to try it.........Jim

[waynelocke]

Brad, that's what it seems to me.

I'm itching to try it too.

[myxpykalix]

I think it would be easier to create a toolpath in PW and follow the instructions under "Turn the blank to a profile"


6666

[jim_stadtlander]

Brad - Just so you don't get confused, Jack's idea of a profile and mine of using what you got already in SB3 is the same idea. I think this would give you an actaully turned object in comparison to Cut3D....I'm guessing on this comaprison(see my thought below).

If you send me the file, can you send it as a DXF file? I have not used STL in Cut3D, so don't know if that works.

It seems with Cut3D you should be able to do the roughing out passes and finish pass similar too Artcam (thinking of it as a flat blank), BUT would the cut file be "trickable"? If this is do-able, Cut3D should be faster and become a turned piece.

---Jim

[blackhawk]

Jim - I can't export the 3D solid file shown as a DXF file. This isn't an option on my CAD software. To my knowledge, DXF only works for 2D data. I asked Tony at Vectric about the .stl files and CUT3D is capable of importing these files. I will email it to you and hopefully it will be straightforward. This piece isn't anything that I need for a job. I was just playing around when I drew this up.

[dana_swift]

Brad- DXF files can handle 3D very nicely. DXF (usually) represents a drilled hole in a solid as an extruded circle. DXF can represent the same hole other ways as well. So DXF files are based on a shape-primitive construction model.

STL files represent all parts of a surface as zillions of flat triangular "facets" each having an "inside" and an "outside" side. The accuracy of an STL file representing a complex surface depends on how much error is allowed to accumulate between the tiny triangular flat areas and the actual curved surface segment it is representing. STL is based on a vector-surface math model.

They each have their advantages for 3D, however STL doesn't handle 2D at all. Both STL and DXF files were created as proprietary file formats, STL has remained nearly unchanged for a very long time which makes support for the format very widespread, in addition it is based on "pure math" so any college vector textbook has all the info needed to understand it. DXF gets a new variant every time a new version of Autocad gets released. Its a "moving target", which causes much importing problems.

DXF "solids" may not be "enclosed" depending on the cad program and what was entered. While STL files are almost always the surface description of all of the surfaces of a solid.

If you use an ASCII DXF you can look to see how much 3D information your CAD program is generating by looking at the file with notepad.

Also STL files can be saved as ASCII so you can look at them with notepad, many CAD programs do not support this version of STL as the files get huge!

Hope that helps-

D

[myxpykalix]

Brad,
In case this has been said in here and i missed it, regarding your part illustrated above, I think you need to stop thinking of the part as being "carved" (even though its round), and think of it like it is being "turned" on a lathe with a gouge only to that specific profile.

[blackhawk]

I noticed on the Shopbot Wiki site that there is a fair amount of indexer info. I found one thread, where Brady mentioned that an indexer video was in the works. That post was in December 2007. I wonder if that is still going to happen.

[jim_stadtlander]

Wayne(or others)--- I am having no luck in working with your equation and the VI, VU commands to work like you guys say. The same old problems keep coming up. Would you be interested in taking this same Cut3D file I made from Brad's model and giving it a whirl????? .......Jim

[rnels]

Have done some testing on Brad's sample.
Created in ArtCam Pro to the specs above (profile may not quite be exact). Created a Z level roughing toolpath and a finish toolpath. If you try these - set your unit values so that if you do a MB 360 it makes one revolution. Use a 3 inch diameter by 12 long already rounded blank and ZZero to the top of the blank zero X at the start of the blank and zero Y in the middle of the blank. Run the roughing pass first then change bits and rezero and run the finish pass. You may need to adjust the move speed per your machine in the .sbp file. I used a .25 end mill for the roughing toolpath and a .25 ball nose for the finish toolpath pass. It could be made smoother and/or faster but just wanted a sample for others to try.

As per above I use the default 13.8889 unit value for B on my prtalpha to get 1 revolution on MB 360. I used default B move speed of 720 on my prtalpha. VD number of axis is 5.

Approximate cut times on my machine - 15 minutes roughing pass, 40 minutes finish pass.

One note the attached .sbp files have a different first few lines of code then the ones I tested with but the code converted to J5 and M5 commands is the same.


6667

6668

6669

6670



Had to put .sbp files on my website they were too large:

http://www.nelsonsdesignssp.com/Nelsons%20Designs%20Download%20Page.htm Brads files.

Randy

[jim_stadtlander]

Thanks Randy--- What I really like is the detailed part of the settings. I was suprised at the the Z being Zeroed at the surface instead of center. I will try that out next week. Also got that post processors loaded and ready to go, that may make all the difference for me.

What Brad needs is to not use Artcam. Somebody out there want to try it like Randy, but instead use a file from Cut3D on an indexer and give a detailed process? This is the real "hang up" area.

Jim

[rnels]

Jim,

My program is really a post processor that will take any .sbp file (not only from ArtCam) that is created in toolpath Shopbot(inch)(*.sbp) format and convert it to rotary. It creates a bunch of other stuff for my purposes but the main part of the program is the converter. You can create an .sbp out of Part Wizard and convert it to rotary. I don't have the Cut3D but doesn't Cut3D output .sbp files?? If the post processors don't work this is another option.

Randy

[scottcox]

Jim,

Cut3D will only raster back and forth across the stationary indexer piece, but you can output a path and modify it as explained below.

I created a profile like this......


6671

...then imported into Cut3d and assigned a raster along x toolpath with an 1/8 inch bit, saving the file to profile.sbp.

I removed one "pass" from the cut file and imported into MS Excel as a text file, parsing the x, y and z into separate columns.

I then calculated that using an 1/8 inch bit with a ten percent stepover, you would need about 100 revolutions per inch of x travel.

So I created a "B" column that reflected that rotation, based on the x value. I changed the M3 to M5, the Y value to zero and output all columns to a .csv file.

I changed the extension and here you have an indexer file from Cut3D.

Not what you expected? :-)

NOTE: I'm experimenting here. Use at your own risk.


Text file
filetoforum.txt (http://www.talkshopbot.com/forum/messages/312/filetoforum-31340.txt) (4.9 k)

Edited to say - You would have to increase your B value limit to 346,000 to run this. I haven't tried that large of a value for the indexer.

[scottcox]

It seems like rotating a model while moving along x, and just varying the z height would be a viable way to carve 3D models on the indexer.

Could any of you write such a beast of a program?

How about it Vectric? A new option for the next version of Cut3D?

[myxpykalix]

Scott...following up on this, while i can see how a "bead and cove" or "hill and valley" profile (like your sample) might might be relatively easy to program just like in the "indexer instructions.pdf" but this cut with a roundover bit is just a matter of position in X,Y and plunge to depth while axis spinning.

I guess my question might be how you might be able to incorporate into probably seperate cut files the ability to plungecut in one place and then rough/finish pass cut your profile?

6672

[jim_stadtlander]

Randy-- WOW!! Am I understanding you properly.
I could take a toolpath that I saved in Cut3D as a .sbp and THEN use your converter that you posted above. It would create a new file that would turn the indexer, instead of the Y motor ?
P.S.-- Cut3D does not give you a choice to save as a rotary file. It only knows X,Y,Z.

Scott-- Sounds like an interesting new approach! But, I am confused on how you come up with the B value of 346,000 ? I want ot try this, but need to know your thought process on that value. In regards to moving the X and Z, the profile device that shopbot has included in SB3 already does this. However it does not permit you to do "fully sculpted non-symetrical carvings, like a cabriole leg with a ball and claw" , so YES, a program for such would be nice.

[rcnewcomb]

In case anyone is unsure, there is already a software utility for the indexer that "wraps" a regular toolpath file around a column.

It is in your shopbot coltrol software under:
Tools/Indexer/"wrap text from part wizard around blank"

It does not need to be text that you wrap around the cylinder, it will accept any .sbp file you have, including 3D tool paths generated in other tool pathing software and it does it in seconds.

It is discussed in this thread (http://www.talkshopbot.com/forum/messages/312/17052.html) <-

[dana_swift]

Scott- "Could any of you write such a beast of a program?"

I write custom programs all the time, what is it worth to you?

D

[rnels]

Jack, you are right from above this would be easier done with a profile - I was just trying to give an example of the roughing and finish passes as I thought they were looking for something. Although this is a base and when doing roughing and finish type toolpaths one would probaby incorporate other detail such as flutes that follow the contours or 3D reliefs, etc.

Jim, it would do that although if you don't have a dedicated 4th axis you may have to do some tricking - but as Randall points out it sounds like everything is covered in ShopBot control software. I will quietly fade away and keep doing my own thing....

Randy

[scottcox]

Jim,

The max b value is 345,600 which equals 12 inches of x travel times 80 revolutions per inch times 360 degrees per revolution.

Here's a shot at the spreadsheet....


6673

and the resulting csv after changing y values to zero, adding the "a" axis values of zero and changing the M3s to M5s.


6674

[scottcox]

Dana,

I certainly won't bear the cost of programming it by myself, but I'm willing to buy such a program at a reasonable cost of $200 - $300 depending on the accuracy and features.

I'm sure there are other considerations, but here's a few to start...

- Roughing pass + finish pass.
- Bit type and size
- How to handle undercuts that can't be seen from Y=0
- How to hold an odd-shaped workpiece from the ends

What else?

[jim_stadtlander]

Randy--Please don't fade away. The more input the better. Just to let you know and all others : This morning I tried cutting the profile method that is included with SB3 and it took longer to cut than your(Randy's) way of doing it, and I don't think more time led to any better results.

Scott-- Now I got it! Guess I was thinking of something entirely differet of the word "value".

Dana-- I just may be contacting you in the future. It will all depend on if I can figure out a "get around". May be if enough of us chipped-in together it could be done?? Scott's list is a good beginning of wants/needs. I think holding odd shaped pieces would fall onto the user's ingenuity. A Possible consideration-- being able to cut past the center point when needed. Would any of this be possible?

[myxpykalix]

Scott...FYI I took your file as posted and changed the txt to .sbp and ran it to aircut the part and it seem to run the entire part without changing any values. It stopped when it looked like it finished. I didn't get any "limit reached" error messages. Would i get one normally or would it just stop?

[dana_swift]

Jim & Scott- rotary indexing is very interesting to me, but I don't own an indexer yet. Parsing/modifying/and generating SBP files is something I already do, so its not a big gap to bridge.

I appreciate your ideas, as that can get put into a generic program and made available when that time comes. Perhaps shopbot would be interested in exchange for an indexer?

Nobody can do custom work for commodity prices, myself included. But 4 axis CNC would benefit me, so I have an interest in writing programs like that for my own purposes. If it can be done generically and re-distributed, so much the better.

As to my general concept.. its how to convert a STL file into a 4 axis cutting file appropriate for a end mill, ball nose, etc.

Thanks for the input-

D

[scottcox]

Jack,

My guess, depending on your move speeds, is that the z axis moved too slowly to notice as it crept along the x with the indexer spinning, correct? Check out the z values in the file. There's just a slight drop (twice).

Also check out the VL command (Value: Limits for table). There you would set the max indexer values, plus and minus, in degrees and file limit checking.

Dana,

I think you should get yourself an indexer! ;-) It sounds like we all may benefit.

Beyond extracting the surface coordinates from a spinning model (?), it's just a matter of calculations to determine bit placement, right? I wouldn't know where to start on that one. :-)

I'm first in line if you write it!

[dana_swift]

My thinking about the problem is to use 2 bits.. an end mill for fast roughing then keep the same bit and mill any "flat surfaces" that are flat relative to the rotational axis by rotating them so the XY axis can mill the flat region. Then change to a suitable ball nose and "drill" the hollow areas that encroach from each appropriate direction. And then mill any other surface.

My thinking is the system is running in a 4 axis mode and "flat" surfaces need not all be in the "rotation axis" just the ones the end mill handles..

Musing out loud-

D

[blackhawk]

Randy - I really appreciate you actually cutting my part out! It looked really great. I am torn on whether to buy an indexer or a spindle first now. Indexer fever is setting in.

[myxpykalix]

Scott,
You are correct that the x axis did creep along however I thought you programmed it that way because it was taking deeper cuts as it went along also, cutting into the "valleys" of the model.

Randy- your "wizard" is more the style of what i think most of us "average" shopbotters are looking for.
When I posted that pic above with the 2 pieces I guess i was wondering aloud about your program in conjunction with simple plunge cuts.
What i think is that like programming different types of cuts on flat surfaces we would do the same on a round object.
So with planning I might set up your program to cut further down the blank and set up some other way to cut the roundover profile as it is simply a plunge down and across the piece.