Indexer PP issue

This is a problem since day 1.
Desktop Max, 6" indexer purchased a couple months ago. Newest version of gearmotor.
FWIW, the instructions to set the step value is wrong in the install instructions. SB calls for 40, which is the old gearbox, but the actual should be 83.3333

When a program is called up, the A & B location changes. The indexer also rotates to match the value.
This pretty much looses the registration, and if makes carving with a rough pass and follow with a finish pass pretty much impossible.
No matter what number is in the Z value, the B will rotate to match.
If the Z is at zero when I start the program, the B rotates to .5 which is the value for Z safe.
Anyone else have this issue?
It is hard to believe that I am the only one.
If you had this issue but fixed it, what was the fix?

Shopbot support has been working on this for 4 weeks now. They think it is in the post processor. Hopefully they will get it sorted out.https://www.youtube.com/watch?v=8Kjm...ature=youtu.be

If the problem happens where your video shows, it's not the post processor, it's their own manual tool change file that is causing it (MTC.spb). Z, A , and B are all being told to go to &safeZ, which is %28, which is the safe Z set in SB3. If they have a machine there that has an indexer on it, it shouldn't take four weeks to figure it out. I don't have an indexer or SB3 anymore so going by your video, that's all I've got. Should be some other indexer users on here to help out.

What do you have as the "home" point for the cut file? If the central axis (the one that doesn't move) home coordinate isn't at zero, then weird stuff happens with the rotational axis.

Why are you using both A and B axis? When I use the indexer, the B axis is always zero. Only the A axis (the indexer) has values that change.

I do not know why your PP is "MTC"... is that necessary? I use SB Arc inch PP even when I am using my indexer. And the 5th axis should NOT be getting any move signal (B axis) unless your machine actually has a 5th axis. Potential solution: Check to see if you can resave with a different PP?

MTC.sbp is ShopBot's manual toolchange script. It is being called up by the actual part file (schwank.sbp) with C9. You could try commenting out the C9 if you have your tool in and zeroed already. That will skip the MTC.sbp.

I see in a preview mode, that if you have 5 axis enabled in VD (values display) that the red position screen has a choice for "indexer" or "5th axis".

Quote:

---

Originally Posted by coryatjohn

What do you have as the "home" point for the cut file? If the central axis (the one that doesn't move) home coordinate isn't at zero, then weird stuff happens with the rotational axis.

Why are you using both A and B axis? When I use the indexer, the B axis is always zero. Only the A axis (the indexer) has values that change.

---

There is no option to select either the A or B.
When I change from 3 to 5 axis as the instructions dictate, both A and B show up.
According to Tech, the A is not used.

Not sure what you are referring to as home for the cut file.
I set all 3 axis to zero before I initiate the program, and as you can see it changes itself.
In this case, I have a point on the machine where I zero the Z, then move it to my Z axis zero point that is a known distance from the fixed point on my machine, then re-zero the Z so that Z Zero is on the center axis.
Reason I used the axis instead of material surface is because my stock varies in diameter.
Note that this happens even when I zero to material surface.
Note that the A and B will set themselves to whatever the Z happens to be. The .5 that it goes to happens to be the safe Z that the software is set to. If the Z happens to be 2 inches, for example, the AB will change to 2 inches.
I installed the PP from a non-tool change machine given to me by the tech and that did not fix the issue.

Another note...when I have the control software set to 3 axis, the Z will still retract random distances when the program is initialized.

My red window does not have those check boxes, it is just as you see it in the video, even when there is no program called up.
I do have the value set at 5 axis.

The PP has the C9 command at the start of the file and again at the tool change.
I assume I eliminate them both?

Since I do not have a tool changer, at a tool change presently the program asks to change the tool manually and allows me to zero the new tool before proceeding.
Will eliminating C9 mean that I no longer can use multiple tools in a part program?

Thanks, I am just repeating what the Tech at Shopbot told me.
They sent me a PP that was supposed to be for a machine without a tool changer, but it did not change the problem, the program still did like the video showed.
What this PP did do, however, was to make it impossible to have more than one tool in my program, so I will have to have a separate part program for every tool.

Closer to 6 weeks now.

>> Not sure what you are referring to as home for the cut file.

What do you have set as the start/home position in the material settings? If you're moving off the 0 point for the indexer, then the rotary axis will do bizarre things.

Post your cut file if you still don't know what I'm asking.

Quote:

---

Originally Posted by coryatjohn

>> Not sure what you are referring to as home for the cut file.

What do you have set as the start/home position in the material settings? If you're moving off the 0 point for the indexer, then the rotary axis will do bizarre things.

Post your cut file if you still don't know what I'm asking.

---

Thanks for responding.
I set the X,Y at zero (use the "Zero Axis box)
The Z in the cut file is the axis, so the Z has to be up high before I can load a part or initiate the program.
I created a new video, see if this helps.
Note also, even though this program had not been run before, and there is no run log, I was not asked if the proper tool was in place.
https://www.youtube.com/watch?v=vOikALiBioo

This is the top of the SBP file.
For some reason I am unable to copy and paste that file here.
Attachment 34364

Post your cut file. The supposed problem is happening when the cut file calls up ShopBot's manual tool change file. If you were to comment out (') those calls in the cut file, how does it run then?

Be sure to do this as an air cut, just in case.

Quote:

---

Originally Posted by srwtlc

Post your cut file. The supposed problem is happening when the cut file calls up ShopBot's manual tool change file. If you were to comment out (') those calls in the cut file, how does it run then?

Be sure to do this as an air cut, just in case.

---

Please excuse the ignorance, I am totally new to G code.
Comment out the call?

I cannot copy/paste the cut file, this forum will not allow it, the paste function is grayed out.
Neither is there an icon to attach a file, only to attach a picture or video link.
How can I post this file?

Choose to reply to thread and in the lower right, click "Go Advanced". Once there, scroll down an use "Manage Attachments" and attach your file through that.

Quote:

---

Originally Posted by srwtlc

Choose to reply to thread and in the lower right, click "Go Advanced". Once there, scroll down an use "Manage Attachments" and attach your file through that.

---

This is the SBP file.
It will not allow me to upload the Aspire file, I get an error that it is an invalid file type.
The Aspire suffix is .crv3d so I changed it to .crv thinking it does not like the "3d" and you could just add it back on, but that does not work either. It tells me that .crv is also invalid file type.

You can change it to .txt and then we can change it back to .crv3d or add it to the extension already there. The sbp file is just a screen grab, so try generating just a one tool file and then open it in the editor like you have there and put an apostrophe (') in front of the C9 and save. Do a find/replace to see if there are any other C9's.

After that, zero out your tool manually like you normally would to start with and run the file (air cut with no tool). If it works/runs as expected, it's not your PP for VCP/Aspire, it's ShopBots own MTC file that is causing the problem. If they can't figure it out from that point, they can send their 6 week paycheck to me and I'll dig deeper. :cool:

Yes, it that C9 is not there, the cut file will not ask you to change a tool, so you'll have to make separate toolpaths.

Quote:

---

Originally Posted by bobmann

Please excuse the ignorance, I am totally new to G code.
Comment out the call?

I cannot copy/paste the cut file, this forum will not allow it, the paste function is grayed out.
Neither is there an icon to attach a file, only to attach a picture or video link.
How can I post this file?

---

So I deleted the C9 command in a part file, and the A & B axis did not change when I started the program.

This solves the problem of the indexer moving when a program is called up.
The downside is that I will have to create a new cut file for each tool in the program, not that big a deal as I typically only have a few tools in a program. At least I can use it now.

Thanks all for the assistance.
Perhaps Shopbot will come up with a fix that will allow for a manual tool change.

Go to your C:\SbParts\Custom\MTC folder and attach the MTC.spb file you have. That is the file that is causing it.

I found these in C:/Shopbot Support/custom/mtc

Just for curiosity sake, what is your B axis unit value set to? (VA, Values Units, B Unit Value)

In both your videos, the MTC script is falling through the "Safe 5 axis" sub when it should be branching to the "Safe 4 axis" sub, which is meant to ignore the B axis.

Meant to reference VU, values units, B Unit Value.

Quote:

---

Originally Posted by srwtlc

Meant to reference VU, values units, B Unit Value.

---

83.3333 is that value.
I had to calculate this based on the motor and gearbox that was provided. The instructions indicated a value of 40, but that resulted in only carving about half way around.
I checked this value using a pointer and a scribed line on a piece of aluminum bar I had, and 360 degree rotation comes as close as my eyes can register.

It rather looks like the Shopbot Techs have given up, so I am on my own.
I get the feeling that they do not sell many indexers for the Desktop Max, so making software work for this combination is not a priority.

It appears that I can make it work by having a different cut program for each different tool I use, and edit each program by deleting the C9 command.

It is a bit of a PIA, but I can manage and it looks like it will at least allow me to use the indexer.

Thank you all for the assistance.

Quote:

---

Originally Posted by bobmann

83.3333 is that value.
I had to calculate this based on the motor and gearbox that was provided. The instructions indicated a value of 40, but that resulted in only carving about half way around.
I checked this value using a pointer and a scribed line on a piece of aluminum bar I had, and 360 degree rotation comes as close as my eyes can register.

---

One way you can refine this number is to turn the indexer 3600 or even 36000 degrees and check the drift.

I'm guessing that they are all working diligently on FabMo, AKA FabNo, AKA NoFab!! :p

Just for fun, lets take a deeper look at this. Replace your MTC.sbp file with this one and see if it behaves the same way when you run an indexer file. If it doesn't behave the same as before, try a multiple tool job and see how it works.

Quote:

---

Originally Posted by srwtlc

I'm guessing that they are all working diligently on FabMo, AKA FabNo, AKA NoFab!! :p

Just for fun, lets take a deeper look at this. Replace your MTC.sbp file with this one and see if it behaves the same way when you run an indexer file. If it doesn't behave the same as before, try a multiple tool job and see how it works.

---

Thanks for the assistance.
I will give this a try and see what transpires.
I am working on a job right now, it will consume my time for a couple days so I will do this as soon as I can.

Reading through some of this thread I will try and clear up some of the issues. First is with the Post Processor. The wrong post is being used. The MTC post will not work with a Desktop or Desktop Max. The correct post can be found C:\SbParts\a_PostProcessors_forCAMsoftware\Vectric Posts\ARCHIVED_VectricPosts\PartWorksPosts\PartWor ksPosts_ARCHIVAL .

The reason the MTC Post can not be used is with a Desktop Max the MTC controls and manages a dual Z the second Z is also controlled on the B axis. The movement you are seeing with the B moving to the same location as the Z is because it is moving the second Z to that location. By using a none TC post this corrects the issue you are seeing.

The second issue is the unit value. For the newest version of the 6" indexer the unit value should be 83.3333. The math to know this is based on the stepper motors step per degree 1.8. The micro stepping of the driver 10 and the gear ratio 15. So the math is 360/1.8 = 200 This is 200 steps in a full rotation. 200 x 10 = 2000 . This 2000 to add in the micro stepping. 2000 x 15 = 30,000 This is adding in the gear ratio and shows that there is 30,000 steps for a full 360 degree rotation. The final is to divide 30000 by 360 to get the steps per degree = 83.33333

The concluded solution:
Use Shopbot_Indexer_X_inch.pp with a MAX
Use a Unit Value of 83.3333 with a 15:1 6" indexer

Hey Ryan, check your MTC file for an error! The reason it doesn't work is that you have a : after a "GOTO Safe_4Axis" on line 254. This causes the IF THEN check for an indexer to fail and allows the execution to drop through to the wrong SAFE AXIS movements for an indexer.

Quote:

---

Originally Posted by Ryan Patterson

Reading through some of this thread I will try and clear up some of the issues. First is with the Post Processor. The wrong post is being used. The MTC post will not work with a Desktop or Desktop Max. The correct post can be found C:\SbParts\a_PostProcessors_forCAMsoftware\Vectric Posts\ARCHIVED_VectricPosts\PartWorksPosts\PartWor ksPosts_ARCHIVAL .

The reason the MTC Post can not be used is with a Desktop Max the MTC controls and manages a dual Z the second Z is also controlled on the B axis. The movement you are seeing with the B moving to the same location as the Z is because it is moving the second Z to that location. By using a none TC post this corrects the issue you are seeing.

The second issue is the unit value. For the newest version of the 6" indexer the unit value should be 83.3333. The math to know this is based on the stepper motors step per degree 1.8. The micro stepping of the driver 10 and the gear ratio 15. So the math is 360/1.8 = 200 This is 200 steps in a full rotation. 200 x 10 = 2000 . This 2000 to add in the micro stepping. 2000 x 15 = 30,000 This is adding in the gear ratio and shows that there is 30,000 steps for a full 360 degree rotation. The final is to divide 30000 by 360 to get the steps per degree = 83.33333

The concluded solution:
Use Shopbot_Indexer_X_inch.pp with a MAX
Use a Unit Value of 83.3333 with a 15:1 6" indexer

---

Thank you for the assistance, Ryan.
Part of our initial conversation right after I got the indexer was that I did, in fact, have to change the unit value, since the value given in the indexer instructions is in error. I calculated the value myself and fixed that issue right after hooking the indexer up.

The only PP available is the one on your web site. There is no mention that this PP will not work with the Desktop Max. Seems like you all would have mentioned that detail, at least note this on the download page on your web site. That would have pretty much eliminated many weeks of back and forth emails.
Also the PP that you recommend will not allow for multiple tools to be used in any part program; Aspire will not even allow me to save a program with more than one tool. This is pretty important information for someone new to the indexer, and should be included in some documentation somewhere I would think.
I appreciate that I am probably one of very few people that have purchased the indexer to use with the Desktop, and that is why you all do not support it.
Unless you all decide to update the PP, I will just use it as it is.

Bobmann,

Did you give the MTC.sbp that I edited/attached a try with your tool change post? I'd be interested to see what it does. As Ryan stated, the MTC file does manage the dual Z situation, but it is also supposed to manage the B axis differently when it sees that the machine is set up for an indexer. Problem is, there's an error in the MTC.sbp that fails at checking for it, and instead, just passes it through to be managed as linear instead of rotary. Give it a try and report back. Who knows, it might work, but there could be more nonsense further along in the tool changing process.

Quote:

---

Originally Posted by srwtlc

Bobmann,

Did you give the MTC.sbp that I edited/attached a try with your tool change post? I'd be interested to see what it does. As Ryan stated, the MTC file does manage the dual Z situation, but it is also supposed to manage the B axis differently when it sees that the machine is set up for an indexer. Problem is, there's an error in the MTC.sbp that fails at checking for it, and instead, just passes it through to be managed as linear instead of rotary. Give it a try and report back. Who knows, it might work, but there could be more nonsense further along in the tool changing process.

---

Thanks, I will try that. Right now I am working on a job with a deadline so it will be a couple days before I can play with the indexer thing again.

Quote:

---

Originally Posted by srwtlc

Bobmann,

Did you give the MTC.sbp that I edited/attached a try with your tool change post? I'd be interested to see what it does. As Ryan stated, the MTC file does manage the dual Z situation, but it is also supposed to manage the B axis differently when it sees that the machine is set up for an indexer. Problem is, there's an error in the MTC.sbp that fails at checking for it, and instead, just passes it through to be managed as linear instead of rotary. Give it a try and report back. Who knows, it might work, but there could be more nonsense further along in the tool changing process.

---

Just to be sure that I will put this modified MTC program in the correct place, does this replace the one that is in my C:/program data/shopbot support/custom/mtc

I am having difficulty location the definitions of all the codes used in the program, for example, "C9".
Is there a list anywhere that tells me what these different designations mean?
I searched for "G Codes" and all I got was designations that were "G-xx"
The software manuals on the shopbot reference page does not define these either.
The SB3 program is no help here, either.
Attachment 34381

Again, thank you for your assistance.

Unless they've changed where it used to always be, place it in the C:\SbParts\Custom\MTC folder and let it overwrite the one that is there.

These docs should help...

https://www.shopbottools.com/ShopBot...mmandRefV3.pdf
https://www.shopbottools.com/ShopBot...%2008%2003.pdf
https://www.shopbottools.com/ShopBot...eShortcuts.pdf

Quote:

---

Originally Posted by srwtlc

Unless they've changed where it used to always be, place it in the C:\SbParts\Custom\MTC folder and let it overwrite the one that is there.

These docs should help...

https://www.shopbottools.com/ShopBot...mmandRefV3.pdf
https://www.shopbottools.com/ShopBot...%2008%2003.pdf
https://www.shopbottools.com/ShopBot...eShortcuts.pdf

---

There is no file path like you describe on my PC.
The custom folder is on the program data folder as I described in the previous post.

I have see those documents, thanks.
Still do not know what "C9" refers to.

I will put the new MTC in the folder that it appears in my previous post, create a rotary part file with a couple tool changes, load it up and report back.

C9 is used in the part file to call up the Custom9.sbc file, which decides what direction to hand off for tool changing. Either ATC or MTC. Since you don't have ATC, it sends execution on to the MTC.sbp file.

Ok, they must have changed where the custom files are stored since I've dropped SB3.

Quote:

---

Originally Posted by srwtlc

C9 is used in the part file to call up the Custom9.sbc file, which decides what direction to hand off for tool changing. Either ATC or MTC. Since you don't have ATC, it sends execution on to the MTC.sbp file.

Ok, they must have changed where the custom files are stored since I've dropped SB3.

---

So, turns out that for some reason the file locations are different on my PC in the house that I use for design vs the PC I use out in the shop to run the Shopbot. The latter has the same files and location as you described.

I put your MTC in place in both computers, and ran an indexer program.
I was able to create a part file in Aspire that uses 3 tools, no problem.
PP used was the "X parallel TC 2016" that I downloaded from SB website.

I started the program, and the B value did not change!!!

The A value did change, but since that value is meaningless in my case, I am a happy camper and just ignore that field.

I will create another part using multiple tools and actually cut a part tomorrow.
Indications are that your fix was successful. I will let you know for sure when I cut a part start to finish.

Thanks again for your assistance.

Good to hear! All because someone couldn't see the errant ":" in the MTC file and take the easy route of "it doesn't work on the Max".

6+ weeks * ??/hr vs knowing what the problem was after your first post.....I'll take the balance $$$ (not from you)! :D

Quote:

---

Originally Posted by srwtlc

Good to hear! All because someone couldn't see the errant ":" in the MTC file and take the easy route of "it doesn't work on the Max".

6+ weeks * ??/hr vs knowing what the problem was after your first post.....I'll take the balance $$$ (not from you)! :D

---

I do appreciate you helping me out here, you stepped in when no one else would.
I created a test part that had several different tools and it ran fine as far as the tool changes go. The B value did do some strange things, but I do not think it has anything to do with the MTC issue.
I will start another thread for that.

I live 20 minutes from SB headquarters, if you are ever in the area, please look me up...dinner is on me.


Regards, Bob