Indexer and ArtCam Pro 2008

[jim_vv]

As you know from "My Indexer" post I have recently connected my indexer to my PRS Alpha 9648. I have mounted it at the end of my machine running parallel to the Y axis. I can turn a blank round with the TI no problem. I have tried to design a leg in ArtCam Pro 2008 and no matter what I do I cannot get it to even air cut properly.

I have tried to design the leg both vertically and horizontally.

When I model vertically and I try to wrap my extrusion in the X axis, it looks right, but the part is off of the material in the 3D view. If I wrap it in Y it is incorrect. I went ahead and toolpathed the 3D view where the leg looked correct (wrapped in X) and then cannot save the toolpath using the Y parallel post processor because it says that the part was wrapped in X.


2802


2803


2804



When I model horizontally and I wrap my extrusion in the Y Axis the 3D view is correct, but then when I toolpath and send it to the Parallel to Y post processor the air cut is not correct.


2805


2806


2807

Is there anyone out there that is using ArtCam Pro and has their indexer mounted parallel to the Y axis that can help me with this?

[steve]

Jim , my indexer is X-parallel. When I want to see what a model looks like I wrap it in Y and haven't had a problem with toolpaths. However you can't easly unwrap the model , I like to see the simulations flat. When I want to see a wraped model now I simulate all the toolpaths and save the relief , open it in another window and then wrap it.My point being , maybe you need to redo the model in a new file and not wrap it at all before you create toolpaths. ... or not!

[jim_vv]

Stephen, I will give it a try. Thank you!

[kg4mon]

I made a new model 12 wide and 36 tall and set a material thickness as 2" and wrapped the model in x direction and I'm getting the same results as Jim did. Just like picture number 2 in the above post. Shouldn't that cylinder be standing straight up with that material outline? I think this is the problem but I've figured it out yet. Hang in there Jim I'm sure help is on the way. Never leave a fallen man behind, it's a Marine thing.

[steve]

OK , maybe I don't know what I'm talking about. I just tried one of my leg models. Was flat , wraped in Y , made toolpath then saved it with Y-parallel... ran fine in shopbot preview. I'll have a closer look at the problem...

[jim_vv]

I just made all of my tool paths on a flat extruded model per Stephen's recommendation. ArtCam will only let me raster in X which is wrong, but I hope that the Y Parallel Post Processor is going to fix that. I'm going out to the shop to try to air cut again. More to follow.

[kg4mon]

Stephen, You and I have our indexer mounted in the x parallel and I'm like you I have never had a problem with the few pieces I have run. But I had never tried wrapping in the x with the indexer mounted in the y until today when Jim called me. So what ever the mistake we are both making it together.

[steve]

Jim , you should be able to raster cut at 90deg. to X ,

[steve]

Rick...nice to have company...

[jim_vv]

I tried to air cut my unwrapped extruded model two ways. I made two models. One vertically in Y and one horizontally in X. For each one I toolpathed a rough Z with a 1/4" end mill, a machine relief with a 1/4" ball cutter (raster in X), and a feature machine (12 lines to make reeds) with a 1/4" ball cutter. I saved them both using the Parallel to Y Post Processor. Neither approach seemed to air cut right.

[steve]

Jim , I did some tests. I did a leg verticaly (Y) , 3d cut with 1/2" round nose. and ran it it VisEdit , seemed to run OK


2808


2809


2810


2811

[jim_vv]

Thanks for your help. I just heard back from Scott at ShopBot. He thinks that I may have an old post processor file. He said that it had been updated so he had me copy a fresh one from the Sbparts/PartWizard postp folder to my ArtCam postp folder. He did say that I need to build my model vertically (along Y) and that the turned ring would not view correctly, but will machine correctly. I have not yet given up!

[steve]

Jim , that would be a handy solution . Let us know.

[jim_vv]

Unfortunately, the freshly copied post processor did not solve my problem. I have tried a Z level rough routine with the default raster and also turning the raster 90 degrees. I get a different result with each tool path, but neither one seems to work. Again, I am just air cutting, but the action that I see is the Z would dig a hole while the indexer moves back and forth like a really short pendulum on a clock. It moves back and forth, but there is no progress. It just stays in the same place.

[steve]

Jim can you send me the .art file? I'd like to try it on my machine.

[jim_vv]

Stephen,

It's on its way!

Thank you so much!

JIM

[myxpykalix]

Refer back to this post, there might be some info you can learn from it that might help.

http://www.talkshopbot.com/forum/messages/33571/37804.html?1242785713

Also "RV" put out a indexer cookbook that had a lot of info on doing this very thing in it but it was 54 megs so it can't be posted here.

[myxpykalix]

jim i sent you soem more info that might help

[khalid]

I did a lot research in Artcam 2008 for producing the quality toolpath for indexing work... After one year of working and many failures I got the FORMULA (Dos & DOn'ts) to get the accurate results via Artcam...In the Following thread, You can see i succeeded in making a Head Post with Artcam 2008

http://www.talkshopbot.com/forum/messages/17997/40694.html?1238978179

In one of my thread at Artcam Forum, I have covered Half of the part (i.e. Only unwrapping the 3D Model) and the second half part was not covered...The second half part include generating toolpath on the unwraped model....

PS:As I will be in Italy (6th june to 24th June, 2009) for 18 days visit with my family...However After coming back probably 26th June , I will able to help in this topic...

[kg4mon]

Could he not lay the model down horizontal in x and wrap it in y, just as if his indexer is parallel in x even though it's not and then use the parallel in x post. But then switch his x and y at the machine, fool the machine. Or am I thinking wrong.

[steve]

I guess I'm missing something. I don't wrap anything unless I need to see how a pattern meets on the back side.
Here is how I do it.
1 3d cut square to round
2 Z level cut
3 3d relief cut with 1/2" round nose
4 turn profile , last pass only


2812


2813

This model was made with the long side in Y axis, the Z level tool path was rastered at 90 deg. I also did three 3d relief paths all rastered at 90 deg. I also did a turning file for Y parallel. all worked fine in simulations. No wraping - except to look at!
2814

[kg4mon]

I'm going to have to try that method. I've only ran my indexer 6 ot 7 times now. I thought you had to wrap it. I'll have some time today to play a little, will post back some results. Everybody does things a little different, that's what make this stuff fun.

[steve]

Rick , I did a whole lot of turnings before I discovered you COULD wrap them. I've done a LOT of turning over the years (28) so I'm used to looking at just a line drawing to see the shape. I started off turning all passes on the indexer but it took too long , the motor got too hot ( I still put a fan on it) and I got tired of all the editing I was doing to cut out all that air cutting on the first several passes.
2815
This is an example , the blank has been turned round , then a Z level roughing cut , what you see is a 3d pass with a 1/2" round nose , the next pass will be a turning pass with the same bit , I would use a 3/16" bit for legs.
2816

[kg4mon]

Now call me stupid if you what to. The z rough looks like the indexer is indexing a degree or 2 or stepover, but we you say a turning pass are you turning the indexer like a lathe? And can that be done in Artcam 2008?

[steve]

I won't cal you stupid if you don't call me stupid LOL.
The Z pass and the first ( and only) 3d pass are with a 1/2" round nose with a step over of .25".
The last "turning pass" is done differently , it is done with the indexer utility "Carve the blank to a shape using a Part Wizard profile" For that you need a toolpath along the vector at 0" depth , this is the "profile " they ask for.
2817

The turning vector is JUST the shape you want and it MUST be centered at 0".
Clear as mud???

[steve]

Man!!! those pictures NEVER go where I want them!!!
It's waaay over there to the right.

[kg4mon]

I forgot about the TI funtion in the shopbot software. Never used it but once to turn a blank round. I kept thinking ARTCAM, you taught me something.

[steve]

Oh yea , the turning vector toolpath MUST be saved with "Shopbor inch" PP

You should all know that I have a talent for leaving out vital little bits of information , so if I told you something and it doesn't work , I probley left something out!

[steve]

Rick , why is it called "TI"? , I just know it as the indexer utility.

I try to use all the utilities and functions... I need all the help I can get...

[steve]

Jim , you up yet , it's lunch time here on the east coast!
You Said "Both files make the indexer spin as
fast as I believe it will go and move Y very slowly." Have you set VD to the right number? for me that's 5 as I have 2 Zs. Could you post a screen shot of part of the .sbp file you tried?

[jim_vv]

Stephen, yes, I am up. I fought with my machine until midnight last night. This morning I have been trying to digest all of the information on this post and your emails this morning. You and Rick have been busy. Thanks so much for your help. Thanks for the part files. I will go air cut the files that you sent to me and report back.

I have 5 axes showing. Axis A reads in inches and does nothing and B (the indexer) reads in degrees.

I didn't know anyone had dial up anymore. Does your phone have push buttons or a rotary dial?

[jim_vv]

O.K. I have just tried to air cut the files that you sent to me.

I set the machine's home at the center of the indexer (my X 0) and 1.5" off the indexer's chuck (my Y 0). I set Z Zero about 2" above my part with no cutter (for air cut).

Here is what I saw when I ran the files:

The .25" roughing file starts off by spinning the indexer as if turning the first section of the leg as Y travels to the first inside radius area. Z then raises and the slowly plunges to rough out the inside radius. While this is happening, the indexer is rocking back and forth like a pendulum on a clock as I described before. Z then picks up and goes to the next inside radius and plunges slowly and the indexer does the pendulum thing all over a again. When done the tool goes home. If I was cutting I think I would have only a couple of slots in my blank.

The relief file moves the cutter in the Y axis nicely as it appears to be rastering correctly. The only question I have here is that the indexer is slowly turning as Y travels so it looks like it will machine the part in a corkscrew pattern. Is this how yours works?

The turning file starts at home and then Z travels up, up, up and alarms out.

I wish I had a web cam so that you could see this. I hope I have written clearly enough.

There must be a setting on my machine that is incorrect.

[jim_vv]

Regarding your TI question to Rick. TI is just the command that brings up the indexer tool. T = Tools, I = Indexer.

[steve]

"I didn't know anyone had dial up anymore. Does your phone have push buttons or a rotary dial? :-)"
LOL :-) , I have to crank it ...

Yea dail up sucks ,dino dail I call it. Supposed to be getting "high speed" in the fall.

That preview you sent me didn't look like I thought it should , looked like the Y moves were in the Z axis . I just looked at the turning file , it's not right. Has your Z axis hit the upper stop yet , I think i heard it.

Just read you new post.

It doesn't sound like any of the 3 files cut correctly. Are you fimilar with the expression "WTF" ?

[jim_vv]

I am stumped. I either have a bad setting (I did everything that is in the manual) or the post processor has issues. I have emailed ShopBot.

[jim_vv]

Stephen, I am sitting here thinking. Did you create the turning file with the Indexer Tool or ArtCam? I am trying to figure out a way to narrow my problem down.

[steve]

I'm not ready to quit on this yet. I got the same preview as you did , which was wrong , I think we are just missing some little thing.
OK , lets start with the Z roughing file. It's wrong , not sure why. It looks like the Y and Z axis numbers are reversed. I'm going to redo it in artcam , gimme a few minutes

[steve]

The turning file was created with the indexer tool with a profile file created in artcam.

[kg4mon]

I'm still hanging in there Jim, Just not much help at this point I've tried everything. Taking some stuff out to my machine to try. Hang in there.

[steve]

Jim , just sent a file , looks right.
X axis doesn't move
Y axis travels down the leg
Z axis goes up and down , but not out or range
B axis goes from 0deg to 1009080 deg


2818

[jim_vv]

Stephen, Very nice! It appears to be working nicely. I am here in the shop letting it air cut the entire file. All seems well.

[kg4mon]

Jim, switching the x and y at the machine works. I took a file that was created in the horizontal and wrapped in y and used the parallel x post. Took that to the machine and set my x,y,z zeros and then VI command switched the x and y and it worked perfectly. This might not be the perfect fix for the problem but it seems to be a fix. I did the x and y switch after I found the zeros so the keyboard function was backwards to what I'm used to . Does this make any sense?

[steve]

Jim I may have stumbled onto something.
What size bits do you want to use for Z roughing , 3d rastering and for the final turning pass?

[jim_vv]

You guys are unbelievable! I am overwhelmed by the amount of time and effort that you have devoted to helping me. Stephen, I have .125, .25, .375, .5 end mills and ball end mills. I was thinking of using .25 end mill to rough and .25 ball end mill to finish this profile.

[kg4mon]

You and stephen seem to almost have this figured out so I will hang back and see the results so not to cause confusion.

[kg4mon]

I just wish I was closer to you.

[steve]

Rick what makes you think I not confused , that last file I sent Jim should not have been right , but it was !!
I just keep hacking away because I want to know what is going on.

Jim I just sent another file but I think it will bounce back , it is 2.4 meg. too big for "dail up"

[steve]

Jim , here are some new vectors I've been using , see any differance?

I don't know If I can mail the toolpaths , I'll try , but in any case the new vectors are the ones I'm using.

[kg4mon]

Jim, hang in there, I got to step out for a couple of hours, we'll check back in when I back.

[jim_vv]

Stephen, I emailed you. Still no luck. The indexer spins and the Y axis moves as if it wants to be outpaced by a snail.

[steve]

In a turning file the indexer should turn ( 360rpm -+) and the Y should move about .01 with each revolution. You can hardly see it move. However in that last Z roughing file I sent the Y axis should be doing most of the moveing and the indexer should only move when Y reaches the end of each cut.
If this is not what is happening then I am at a loss to explan why.

[jim_vv]

The turning file did exactly as you described.
The other two files (Z Rough and Machine Relief) were made in ArtCam, right?
Is it possible that there is something up with the post processor when it is used with ArtCam? I believe that it is the same one that the Indexer tool is using for the turning file.
I don't know what to say, but "Thank You" for your efforts.
I have yet to hear back from anyone at ShopBot.
Perhaps I should just temporarily switch axes like Rick suggested.

[steve]

Here is a shot of what the turning file should have done , although it may have taken more than an hour to do it.
2819

[steve]

The vector for the turning file uses adifferent PP than the other files. It may be the PP , I going to think on it for a while , must be an answer.

[myxpykalix]

A couple suggestions. If you want to send the file to me to have a look i can try to help. The more brains you have thinking on it the better. Also most times a picture is worth a thousand words so i can take a video of it and post it on youtube.
Regarding posting pictures so they line up underneath each other, here is how you do it.
popjpeg{42691,}
popjpeg{42692,} (the \ is missing before each)

so you attach 1st pic then go to next line, add next picture, then it looks like this


2820

2821

Instead of adding them on the same line like this
popjpeg{42691,}, popjpeg{42692,}

[myxpykalix]

"Here is a shot of what the turning file should have done , although it may have taken more than an hour to do it."popjpeg{42691,}

or adding them to the same line after your text

[kg4mon]

Jim, I played with this some more sense I've been back and drew up a model in the vertical and DID NOT wrap it, just toolpath with raster 90 degrees and used the parallel y post and it work perfect!! So my conclusion to this problem and I may be wrong, it's not the pp it's artcam in that it lays the model off the material instead of vertical. I think ARTCAM needs to get involved with this matter. There may be a setting we're missing, a glinch, or something. The software won't even let you mirror the relief vertical it just does nothing. What ya Think?

[kg4mon]

I'm Back Jim, Had to go eat with the family, Just tried to return you call.

[steve]

Jim , I looked at the PPs and they look OK however they don't act the same , so I don't know enough about them to make changes. I do think there is a problem with the Y parallel PP. I did some tests , I'll try to get the pictures in order.


2822
this is the Y pp "as is"



2823
this Y axis toolpath was converted by me from an x toolpath



2824
this is the X tool path I changed , you can also see the Y cut , they are the same.
I think this is an Artcam problem.

[jim_vv]

Stephen, Thanks. I tried the file that you most recently sent to me. The indexer spins and no other movement occurs.

[steve]

Jim , I tried that file and it works. As well as a PP problem their may be a problem with your machine , maybe with the axis assignment? That file should send the Y axis down the length of the blank and back while the indexer should only turn about 8deg. when Y reaches each end. If this is not happening , something is up! Look at the file , by the numbers, that's what it is supposed to do.

[myxpykalix]

Stephen,
What version of the control software are you using? They recently wrote in A,B moves translations in the newest version for the indexer and that may play a part in some of the problems you are having.

[steve]

Jack , I just down loaded the latest version of control software. Unless they ( shopbot )changed how instructions are read , that last file works. Here is a shot of part of it.

2825
As you can see :
M5, = move 5 axis
, = no X movement
15.311317, =move Y to 15.311317"
-0.26845 = move Z to -0.26845"
,= no A movement
0.0000 = move B to 0.0000 "
As you can see Y moves from 15.3... to 22.948187 , then B moves to 8.5721 deg. and Y starts moveing towards 0" again. That is the raster movement .


As I understand shopbot files these are absolute instructions. If the machine is not following these comands there is something else going on , not the fault of the file.
If I am wrong I will be happy to admit it and need to know .

[myxpykalix]

sometimes we overlook the obvious. Do you have your B axis setup in "degrees" instead of "inches"? Send me the file if you want and let me take it out to the shop and try it on my indexer and see what happens.

[steve]

Jim , I got the first 8 pages alright! Anyway they use a different method than I do. I do as many turnings on my CNC as flat work , the work top is used mostly to hold turning blanks. Actually the indexer was half the reason I bought another bot. If it didn't have it I would have gotten something else!
My method came about by trial & error , more error than trial I guess , but mistakes are where we learn the most.
I don't use the "zero plane" method , My page is set to the full size of the blank I am turning , that is , a 3.5 x 3.5 x 29 3/4" leg would require a page size of 10.9955 x 29.75. I do whatever work I need to do , when it comes time to model in 3D and tool path I set the material at half the blank size ( 1.75") and make sure the off set is at least .01. That way I know the relief will be cut .o1" below the surface. In short ( if I understand correctly) the "zero plane" method measures the model from the bottom up and my method measures the model from the top down. I don't know that my way is better , I only know it gives me what I need.

all of these turnings were done that way

2826


2827




here is an example of a interesting mistake
the neck is far to small for a table pedistal , but OK for a lamp1

2828

Anything that can be done flat can be done round.
2829

[myxpykalix]

absolutely beautiful stuff stephen. You need to give a class on how to do all this...very cool!

[steve]

LOL Thanks Jack...when and where?
Actually I think Brady Watson is doing a video for indexer stuff. His instruction will , I'm sure , be much more technically accurate than mine. I just keep banging away until I figure out what works.
Here are a few more.

2830

[kg4mon]

Beautiful WORK !!!!

[scottj]

For those following this thread here are the new versions of the Post Processors that I sent to Jim. He tells me all look good so far so if you find any issues Please let me know. THESE WILL NOT WORK IN PART WIZARD (sorry but they are only for the 3D software packages)
Post Processors for the indexer-
Shopbot_Indexer_Posts.zip (http://www.talkshopbot.com/forum/messages/33571/Shopbot_Indexer_Posts-42794.zip) (4.6 k)

[myxpykalix]

I'm not holding my breath waiting on his video, as he says "it will be done when its done". I'm sure he has more important things to do.
If you didn't live way up in canada i'd come knockin on your door. Where is nova scotia? Is that on the east coast, west coast?

[br928]

Scott,

Are these Post Processors for Aspire?

[steve]

East coast Jack.
Maybe I should do some videos? or at least some PDFs on how I do this stuff.

[myxpykalix]

I sent you an email to your profile address stephen

[myxpykalix]

someone was having a problem with the X/Y post processors and i don't know if this would work and this may have been included for a while and i just didn't notice it but in the newest version of the control software (3.6.1) in the shopbot fart pile toolbox there is a utility named "XY SWitcher" and i wonder if you couldn't use that to correct your X/Y issues? Just grasping at straws here...this may not work at all.

[myxpykalix]

correction--"Shopbot part file"

[Brady Watson]

Yes...Don't hold your breath on the video. Between work & planning our wedding, there hasn't been free time to develop this. Contrary to what some think, creating a video good enough to cover all the bases, takes a tremendous amount of time and energy. If you have the time, energy and inclination to do something - GO FOR IT!...and then YOU get to answer a flood of emails for free!

-B

[steve]

Brady , first of all congradulations on you wedding!
Secoundly , all those emails ...hmmmm , maybe I will just offer those services on my web site. I suppose you have to allow for some instruction time in the price.

[jim_vv]

Halleluja! After getting the corrected Shopbot_Indexer_Yparallel_inch.CON post processor all is well.

A big THANK YOU!!! to all who have helped me. I have learned a lot through this process and I believe that I have have made some new friends as well


I thought that I would share the method that I tried.

Here is a screen shot of the vectors in ArtCam (I modeled vertically because my indexer is parallel to Y)


2831

I then extruded my vectors


2832

I then wrapped the extrusion in X (this view seems odd, but it does machine OK)


2833

I then chose a Z Rough toolpath (raster 90 degrees)


2834

I then chose to machine the relief (raster 90 degrees)


2835

I then chose to add a couple of feature machine toolpaths for some lines on the part


2836


2837

I then simulated all of the tool paths.


2838

Here is my 3" redwood blank after the Z Rough with a .375 cutter


2839

Here is the finished part after all of the machining. The leg is 3 inches in diameter and 24 inches long.


2840


2841


2842

Here are some notes that I would like to add.

Machine Times:
Z Rough, .375 endmill(15 minutes, 38 seconds)
Machine Relief, .25 ballmill (2 hours, 22 minutes)
Feature Machining .25 ball mill, .08 deep( 2 minutes, 48 seconds)

I had a little trouble when machining the relief. The machine stopped moving a couple of times, but the display kept showing movement. I had to stop the machining and zeroed the indexer and then restarted the machining. I think this may have been because my Y carriage is really close to my X proximity sensor. I moved the sensor a little, but am not sure if that solved my problem.

Another thing that I tried was to see if I could speed up the machine relief process.

My original toolpath used a .25 ball cutter at .015 stepover. I redid the toolpath about half way through and changed the stepover to .025. The .025 did leave small lines, but I think that they are sandable. The .015 finished like glass!

I should have changed the feed rate on the feature machining where the two lines go around the center of the part. The indexer spun way too fast to give me a good finish across the grain.

I will be forever playing with feeds and speeds!

Again, THANK YOU to all!

[kg4mon]

Looks perfect Jim, Congulations!!! Job Well Done

[myxpykalix]

A couple questions jim...
When you make your flat model the width that you make it should equal the radius of the blank you are using correct?

Also it looks like your Zzero is at the center of the blank but also at the head of the blank located at the headstock?

2843

[jim_vv]

Jack, My model width is the diameter of the part multiplied by 3.142. 3" x 3.142 = 9.426 (I actually went 9.44 because the Wrapped view showed a tiny unmachined fin). The material is 1/2 the diameter and Z zero is bottom of block. Zero the machine at top of your blank. Your orientation text on my simulation is correct except for the width text.
2844

[jim_vv]

I just noticed that my previous pictures show the material wrong. Can I edit a previous post? If not I will follow with revised screen shots. Sorry.

[jim_vv]

Guys, I am so sorry. I noticed that my 3D toolpath previews this morning's post show the material located in relation to the part incorrectly.

Here is the revised Z Rough


2845

Again, I apologize.


Here is the revised Machine Relief


2846

And the revised Feature Machining


2847

[myxpykalix]

Ok, so let me see if i understand...
"my model width is the diameter of the part multiplied by 3.142. 3" x 3.142 = 9.426

So using that equation of "pi" to calculate my "width" I first measure my diameter and make my width of the model the results of the equation like in your example above?

So using that in this example:
2.75" diameter X 3.142= 8.64" is this correct?

So the idea is you fit the model to the material?

So what if someone sent me a model that was 8.64"
(just using width in this example so as not to confuse) and i did not know I was starting with a 2.75" diameter piece. How can I take that 8.64" width and back figure what my diameter would be that i would have to cut my 3" square piece down to, to be able to have this fit?

This is one way i learn is by taking the example the teacher gives you, do your figuring, then have the teacher affirm that you are doing it correctly.
So teacher do i earn a gold star?

[jim_vv]

Jack, You get a gold star! Circumference equals Width or Height (depending on what axis your indexer is mounted parallel to). Think of it the way Stephen described how he does his. He does all of his work flat. I think he has a good technique!

[jim_stadtlander]

Jack,

8.64" Divided by "pi" 3.142 = 2.749.... Or a model 4.5 wide would then be for a turning 1.432 in dia.

[myxpykalix]

Jim,
"8.64" Divided by "pi" 3.142 = 2.749"
2.749 is close enough for me to 2.75 or good enough for government work, for sure!

".... Or a model 4.5 wide would then be for a turning 1.432 in dia."
I'm not sure i understand what you are saying here.
EDIT.i did the math...i get it..thanks!