New Rotary Set Up

[exapprentice]

Hi every one
New year is nearly here and I am getting restless with too much time on my hands during the holiday!!!
so new year - new project? me thinks

New Rotary attachment.
my intention is to build a rotary attachment to cut both round and square tube.
My machine runs on CandCNC MP3500 ethercut, which will give me 5 independent axis in total, I am using 4 for my table that leaves 1 for my chuck drive
so this is the early stage of planning and my first question is - what is the ideal RPM I should be aiming for on the rotary axis

Only guesstimating but I would think my tube dia would be max approx 150 mm (6") and the minimum dia around 40 mm (11/2") same for the box but adding in 100 x 50 mm (4"x 2") rectangular section, wall thickness from 2.5 mm (3/32") up to 10 mm (3/8")
I have sourced a self centering 4 jaw chuck so the first stage will be some form of gearbox to mount motor and chuck but I am going to need an additional stepper and driver and maybe a new power supply hence the RPM question.

Just thinking allowed I will post pics of the build during its progress so everyone could benefit (if your thinking also about a rotary axis)

Am I right in thinking I should base the rpm on achieving my fastest cut speed required on the smallest diameter to be cut and work back through the gearing to the optimum stepper RPM
Allowing for the unknown future requirements lets base it on a material thickness of 0.9 mm (0.0354")mild steel CR = 9652 mm/min (380"/min)
using my existing PM 45 & machine torch (that is pretty much worst case, I believe )
In my reckoning that means about 77 rpm top end

looking forward to dialing it all in (I think )

[Thor]

I would figure your 1-1/2" min diameter tube as 14 ga or so, so that means 200ish ipm. On that size then you would want 42 rpm. I would probably shoot for 50-60 rpm top speed just to maybe do some 1" tube

I need to get busy and finish my rotary axis build as well, but mine is more like max 16" dia, but probably still shoot for the same 60 rpm or so max rpm.

[acourtjester]

I looked at this in a different way I used a stepper motor for the rotation drive and calculated the steps per inch for the tube/pipe diameter and just used the normal IPM for the thickness of the metal cut. This way the speed across the metal surface was the same as for flat sheets.
http://www.plasmaspider.com/viewtopic.p ... er#p106713

[Brand X]

Lets say you use a 620 oz stepper motor.. What gearing would get you to where you want to be? Just a general overall good average. It's all over the board, from what I can tell.

[exapprentice]

OK I have been thinking a little more about my initial setup. I am pondering the inertia involved if I use the 4 jaw chuck
Maybe fabing up my own light weight 2 jaw chuck would be a better option and would allow the drive to respond quicker with less mass to deal with.
As far as the gearing goes I am thinking around the 3 - 4 : 1 range
That should be about 200 rpm at the stepper ? Might ponder and go up some more on the ratio

[exapprentice]

Still Thinking (not doing - yet)

going back over my initial thoughts, if I only want to do round tube that all seems pretty straight forward, the mechanical's are the same but the Z stays over the centre line of the tube so either the X or Y becomes the rotary axis using the same driver and motor just plugged into the new rotary (chuck)axis while tube cutting, with this option I could use the "Pipe Wizard" software

Cutting square tube is becoming a little more difficult as I would need to have to be able to have 4 axis of simultaneous motion XYZB
(B = chuck / rotary axis) for this I believe I will need to get SheetCams Rotary plugin and POST

Has anyone used this plugin & Post with a MP3500 ethercut and std CandCNC screens, where do you set up your "B" axis (I assume in Mach) and the post then calls for the rotary in the code as part of the cut profile

[steel 35]

Still Thinking (not doing - yet)

Has anyone used this plugin & Post with a MP3500 ethercut and std CandCNC screens, where do you set up your "B" axis (I assume in Mach) and the post then calls for the rotary in the code as part of the cut profile

YES ^
I have the Precision Plasma 25:1 worm gear reduction Acc, 620 stepper (Have used not proficient)
I am working with the post processor for the B Axis. The set up is like you mention, In the Mach motor settings.
To activate the rotary Use that Post Processor In sheetcam If you find a Screen that will allow you to use the torch however let me know
I have used the switch box that came with my Plasma. Have gotten some very nice cope

Wish I could drop the $ for the Pipefit.

[acourtjester]

Giving some though about your questions I assume you are looking at a 4th axis to rotate a square tube and then do normal axis movement for cutting on the flats. If that is the case why not just have the B axis as a stand alone and use a separate G-code just to rotate it 90 or 180 degrees then resume your cutting action. In Mach you just use the pins for B axis and hook them to your driver.

[exapprentice]

Hi Tom & Steel 35

Thanks for your feed back

I am looking at trying to get to a set up as you can see in this you tube clip:

https://www.youtube.com/watch?v=d2fscbLNtGU

I would like the facility to cut around the corners of the box section tube (I have a few ideas on products that would need this ability)

Steel 35 I agree about the cost of the pipefit but when I purchased the MP3500 I went balls to the wall and bought a lot of kit and software as a package from CandCNC saved for ages and then went for it to get the biggest bang for my money at the time
Glad I did, it all seems to work well for me (so far)

[steel 35]

Thanks for sharing the video!
If building your own think about the water flow through the chuck as Orge has done the smoke is hideous. Pretty sure it improved other aspects as well.

[acourtjester]

Seeing the video it is good you have the MP3500 to get the quick Z action to follow the odd shape rotating much different then with round tube. If you are just cutting on a standard square tube I would make up a flange to couple with the tube and not use a 4 jaw chuck. The current flow through the scroll of the chuck may not be good for it.

[tcaudle]

Wish I could drop the $ for the Pipefit.

A lot of people misunderstand waht pipefit is: Is a DESIGN plugin for SheetCAM. It less you define simple of complex pipe joints shows them in 3D and then generates the "Contours" in a flat 2d plane to use in SheetCAM. It does not do the " wrap " of the 2D around the pipe ...taht is done by the Rotray Wizard (free) and a custom POST So if you can do the shape of the cut and the math for the cuts in 2D then you don't need Pipefit. In fact you can use the lower cost rotary plug-in from SheetCAm and it also does sqaure tube. It won't draw the weird shapes for you butit will cut anything you can draw. I belove there are some free programs that will let you put in pipe sizes and angles and it will generate a 2D drawing you can print out. (actually made to wrap around a pipe as a template ) but you might be able to trace it and transfer to SheetCAM for branch pipe cuts.

[steel 35]

This is the program I have used it works great, saves as PDF; worked very good but still never got the torch to fire Through mach and wondered if it was partially because of a licence thing?

http://www.metalgeek.com/static/cope.pcgi

[acourtjester]

Ok Steel35 that seems to a simple fix I just did a test with it I downloaded a G-code file from the site (click on the Red G-code below download pattern). I then loaded it into Mach 3 and all the X & Y values are there. Just edit that G-code and add the normal cut start (position start location and touch off and pierce and M3 and delay then drop to cut height) at the top of the G-code supplied and it should work fine.
Thanks for posting that site info

[exapprentice]

Hi Steel 35

Please can you give a bit more info when you say:

"To activate the rotary Use that Post Processor In SheetCam If you find a Screen that will allow you to use the torch however let me know "

Are you saying that if you use the rotary post in SheetCam to produce the "TAP" file then it wont load into the std CandCNC profile screen? or any other to run the TAP file

I really need to understand this bit as its fundamental to how I thought it worked I thought you could just load the TAP file as per any other TAP file into the std CandCNC run screen / profile

[steel 35]

These do produce a tap file and load into the screens as usual!

I Had to delete a few lines in gcode that caused pauses

The screens have there challenges, Partially me?

[steel 35]

Mine cuts very well but wish the run button worked instead of this, & Hoping to help the divot as well

[exapprentice]

Hi steel 35
Thank you for replying to my question. Did you purchase your rotary post from SheetCam and import it into your set up
I suppose the next question to anyone else out there using this rotary post is this a common problem:?:
If it is has any one asked Les at SheetCam for a fix
Does the rotary post have the option to set your switch off set
I know loads of questions, sorry, just trying to sort things out in my head before jumping

[steel 35]

Look on the disk from c&cnc in the pipe wizard section, Looks like 4 rotary post processors from them in the prior screen shot! put that with maybe three screens and there are a lot of combinations. I am sure one can work flawlessly just haven't found it; nor got a nudge in the right direction.

My only problem may come from the fact I am using a post that starts with DTHCII Might be one pin / port setting?


Experiment on that SQ tube theory and get back soon.

[acourtjester]

I try to keep with the “KISS” method when I built my rotary cutter I switched the motor output for the standard X stepper and moved it to my rotary stepper motor. I then just used standard post processor in sheetcam to plan the cut. Using the program Steel 35 posted will give you the file needed to generate the cut profile. The only thing needed was the pierce and cut info. Now I am only talking about round shapes not square.
https://www.youtube.com/watch?v=mDO9sx8NiPA

[steel 35]

This is where I would start if I was attempting again today. I didn't find the little detail how to set the rotary Axis before.

[_Ogre]

google ''longworth chuck'' and modify it using steel cut on the plasma table
http://www.woodworkersguide.com/2010/10 ... rth-chuck/

we only have a 3 jaw chuck for the self centering feature on round tube
using the longworth chuck you could could use 4 or 8 grips to grab square tube and it self centers for round tube
this chuck won't support much, you'll need tube supports for any long tube

we do mostly 2.5'' and 3'' 16ga ss round tube on our rotary head
3'' tube has a 9.5'' circumference, at 90 ipm you'd need 10 rpm
thicker wall tube would cut slower obviously
i'd think you'd need a max rpm of 10 to 15

this is cutting a 3x3 cope in ss tube
https://www.youtube.com/watch?v=Ilc_ldF7eLE

[Thor]

I'll have to get pics of mine up when I finish it, but I went with a 4 jaw self centering chuck with 2 piece jaws. For round and square tube use the standard jaws, for rectangular tube, make 2 new top jaws with large V grooves in to grab tube by corners, would work on square tube too.

[exapprentice]

Ok - Just a quick up-date

I have now purchased the rotary plugin from SheetCam, done some CAD work and knocked out some simple test files (for square tube).
I have installed the license and have been able to run these test files through the SheetCam simulator and all is looking good

I am struggling at the moment trying to work out the axis orientation in the simulation as it is running to match them to the orientation that I want to set up my tube cutting attachment on my machine, I am sure I will grasp it soon (early days yet)

I am now turning my attention to the mechanics of the attachment, trying to come up with a set up that has minimal mass to minimise the inertia requirements of the rotary axis, hopefully to achieve a smooth, responsive attachment capable of holding round, square and rectangular profiles, should be easy, compared to what I know will required in the next steps of actually producing good product.

I did acquire a 150mm (6") 4 jaw self centering chuck, but the weight is 9Kg (20 lb) so I am now pondering that that mass is a high + the rest of the gearbox internals so the "smooth, responsive" part of my design spec might be under question
I am now re-considering my first thoughts of "fabing up my own light weight 2 jaw chuck" would be a better option, more work short term but maybe a better long term answer

As per my other posts I will as time goes along, post pictures and updates as things progress, but I do intend sitting back in a comfy chair, visulising the build and maybe a bit more pondering with a mug of tea (a very British way of working things out )

I am also in the process of trying to build my own powder coat oven, heated via an indirect oil fired space heater which is probably more fundamental at the moment to my business

[_Ogre]

trying to work out the axis orientation

my axis's are reversed from flat cutting, i just deal with it

for round tube copes i use the cope calculator from cobratorch.net and download into dxf
then load into autocad and modify/massage it from there

give us some feedback on the rotary plugin for sheetcam
the plugin came out after i got use to other methods