Pulse indexer programming

[Metals and materials]

Hello all, 

Thank you in advance for taking time to read and answer to my question.  I am new to Mastercam and learning all day, everyday!

So, I have a PROTRAK SMX controller, Mill from southwestern industries and a pulse indexer from HAAS! And they are all attached together and working. 

Question is: How can I program from Mastercam to pulse the indexer. We have few programms that works like: 1) The program is run 2) pulses the indexer 3) indexer rotates & parallelly program waits for pulse back. 4) when pulse is back, program runs again. 

Now, I do not know how to make the program so that it can give pulse to indexer. Untill now, I figured to use M21. I can just edit the program manually and edit in mastercam code expert, just a simple line M21 ( I have not yet checked if that is the code that will work in southwestern) but I was thinking if there is a way to do it in mastercam automatically. 

 

Thank you, Again!!!

[AHarrison1]

You could use Manual Entry and add the M21 that way.

 

Also, check with your re-reller to see if the pulse indexer is supported.

Edited July 27, 2023 by AHarrison1

[Leon82]

we use the manual entries with the required m code when we did it.

[David Colin]

I’ve got some VTL machines with indexer on X axis. Post is customized to spit M code instead of A value. Value is post in a comment. 

It's all about machine definition and post. It should be easy to tweak it, share files if you need help.

 

[Metals and materials]

 @AHarrison1, yes, I checked with them. Pulse indexer is supported. 

@Leon82, Okay. so just put in M21 when we want to pulse index and that's it. 

David Colin, for security purposes, I cannot share the file. Do you have any links, where I can refer to tweaking the post for that?

[Metals and materials]

Okay, so I am trying to add M21 lines. Question is where? I have a cylinder with 4 holes at an angle of 90 degree. Top hole is in the top plane. As my 3axis mill does not have in built rotary, I am not able to rotate the part. I am trying to unroll, drill, add M21 to roll. but the drill toolpath is not working at all. This is kind of confusing, but if anyone have used pulse indexing programming on cylinder or something like that with 3Axis mill (I have protrak but any 3 axis is fine), if you can share a file, I can take a look and will make everything a lot easier and lot helpful. 

[crazy^millman]

You are over thinking this. Create the operation in Top. Then use Transform Rotate to rotate it 3 times 90 degrees with Right being the Control Plane for rotation and done.

[jpatry]

On 9/1/2023 at 8:26 PM, crazy^millman said:

You are over thinking this. Create the operation in Top. Then use Transform Rotate to rotate it 3 times 90 degrees with Right being the Control Plane for rotation and done.

He doesn't have a rotary axis, he only has a rotary indexer where the rotational movement is stored in a separate program inside the control box attached to the indexer.

He needs gcode in machine control to ping the box via the M21 output signal, whereupon the box will advance the indexing program one step and return ping the machine control to allow the program to continue.

 

Cave man simple solution is most probably just building a manual entry with the requisite safe moves.

[David Colin]

@jpatry Your machine has an indexer but to program it in Mastercam you need to add a 'virtual' rotary axis to your machine definition. Then make your post spit M21 code and whatever you need. You even can make your post create another file with all values you will need to input in your indexer NC.

Here is an example with machine/post included (just for example purpose, don't use that for production)

Indexer example.MCAM-CONTENT

[crazy^millman]

10 hours ago, jpatry said:

He doesn't have a rotary axis, he only has a rotary indexer where the rotational movement is stored in a separate program inside the control box attached to the indexer.

He needs gcode in machine control to ping the box via the M21 output signal, whereupon the box will advance the indexing program one step and return ping the machine control to allow the program to continue.

 

Cave man simple solution is most probably just building a manual entry with the requisite safe moves.

Good point and thanks for giving thought to this issue they are having. To get the Mastercam file to verify the part a programmer will need a method to do it. I gave a method to accomplish that task. M21 with the angle output can be like mentioned with manual entry, but what good is a programmed file if everything is only represented in the top plane and not at each indexed position?

David has given some insight lets see how it used and if more questions are asked. Then from there we can see how to help them learn more about to use Mastercam in this setup.

[Metals and materials]

Good morning and happy Labor Day! I was out yesterday. 

But, this is very good insights. 

@David Colin I have 2023 version of mastercam. FIle is of newer version. So, i am not able to open it. 

@crazy^millman To prerform transfer toolpath I must have atleast one toolpath. But, 

I think I stumbled upon another problem while trying the method above. Made Top plane, created curve all edges. Hit the drill toolpath, time to select hole --->but I cannot. I am guessing the cylinder is round. so the holes are not flat but curved and that is why mastercam is not picking up those holes. 

here is the screenshot of what is happening. 

I found this post online------  

 

 

I understood verisurf is the way to do this so downloading the tools and hopefully, it will be resolved. 

Also, I am very new to mastercam, so I apologize for this all-small issues. But I am quick learner. Hopefully, in the future, I will help others as well. 

 

 

[David Colin]

@Metals and materials Here are 2023 files

Indexer example_2023.MCAM-CONTENT

[Metals and materials]

Perfect @David Colin. Thank you. Let me take a look at this.

[Metals and materials]

@David Colin So you used Toolpath transfer option to rotate it. Whenever the tool rotates, we just put 'M21' there. Makes sense. 

I am still doing that drilling operation. Once that is done, I will come back here. 

[David Colin]

@Metals and materialsYou can use toolpath tranform (by plane) or set any Tplane in your operation toolpath

[David Colin]

2 hours ago, Metals and materials said:

Good morning and happy Labor Day! I was out yesterday. 

But, this is very good insights. 

@David Colin I have 2023 version of mastercam. FIle is of newer version. So, i am not able to open it. 

@crazy^millman To prerform transfer toolpath I must have atleast one toolpath. But, 

I think I stumbled upon another problem while trying the method above. Made Top plane, created curve all edges. Hit the drill toolpath, time to select hole --->but I cannot. I am guessing the cylinder is round. so the holes are not flat but curved and that is why mastercam is not picking up those holes. 

here is the screenshot of what is happening. 

I found this post online------  

 

 

I understood verisurf is the way to do this so downloading the tools and hopefully, it will be resolved. 

Also, I am very new to mastercam, so I apologize for this all-small issues. But I am quick learner. Hopefully, in the future, I will help others as well. 

 

 

About hole selection, if you have issues to select autocursor locations you can use 'hole axis’ command in model prep tab which allow you draw center points or lines. There is also another process using 'find hole' to create hole solid feature.

[Metals and materials]

@David Colin I am unable to select holes in the operation. Small holes, Mastercam can figure. But little larger like the middle big hole shown in the above picture, Mastercam is not able to figure that out.  

[Leon82]

modelprep, hole axis

[Metals and materials]

Yep, that is what I am using. Mastercam is detecting small holes. Bigger one is not detecting. 

[crazy^millman]

27 minutes ago, Metals and materials said:

Yep, that is what I am using. Mastercam is detecting small holes. Bigger one is not detecting. 

Split hole turned on? Is is a hole or a conic? .001 degree taper is not a hole it is a conic.

[Aaron Eberhard]

Can you post your model up?  It might be as simple as choosing the solid face of the hole instead of trying to snap to an edge.

[Metals and materials]

@crazy^millman   @Aaron Eberhard

Here is the program.

3AXIS_with_rotaryIndexer.mcam

[crazy^millman]

39 minutes ago, Metals and materials said:

@crazy^millman   @Aaron Eberhard

Here is the program.

3AXIS_with_rotaryIndexer.mcam 987.12 kB · 1 download

Like I said originally that was shot down. What good does it the programmer is everything is from top. There are some planes made correctly just not picked correctly for the operations. I would name them different than Front-1 to Front-1-1-1-1-1.  You need to make planes for each hole Then work from there. You have everything in TOP and then try doing a transform of that. Not best practice.

The large hole is small conic like I said not a true solid hole so you have to make a decision what do you want to make it?

If it were a true hole we wouldn't see the overlapping entities when looking down from the top view. Garbage in gives us garbgee out. Whatever CAD created this has not got the tolerance set correctly for file conversions. Probably .005 tolerance verse .0001 it should have.

What do I know????

[Metals and materials]

@crazy^millman This is so helpful! Used dynamic milling and the big hole is done as well!! 

Finally, this is what I am doing right now. At Rotation, I am just writing M21. And that will do it, correct?

 

My first rotary indexer programming!!!!

[crazy^millman]

15 minutes ago, Metals and materials said:

@crazy^millman This is so helpful! Used dynamic milling and the big hole is done as well!! 

Finally, this is what I am doing right now. At Rotation, I am just writing M21. And that will do it, correct?

 

My first rotary indexer programming!!!!

That should work, but again make sure your planes are correct for each operation. You could get a post dialed in to do al of this without the need of manual entry.