Here we go again . . . MK4

[routercnc]

Thanks Tom. Yes, lots of ways to drive 2 ballscrews - that one would work as well.

Your little machine looks really good. Nicely built !

[routercnc]

OK, more updates. To finish off the info on the bed rail supports, here is the little jig I made up to hold the bosses in place:


Here it is in position:


It uses 6mm shoulder bolts to give a good reference position and picks up off the inner tapped hole already there. This holds the boss in just the right place for welding. It's now ready for welding - just need to catch my friend with the welder in the next few days or so. This is bolt down the supported rail which obviously uses a pair of bolts on either side of the flange.
I've also taken the opportunity to spot out the holes for a profiled rail (i.e down the middle) to make a future upgrade much easier to do.


Next up are the end plates which hold the motor mounting plates. Starting with a nice skimmed off the sacrificial board:


Then setting up:

(note that I've scribbled down the X, Y, Z coord of the workoffset on the drawing - I always write them down in case of power failure)

I'm making a mirrored pair here. A few holes, and a large pocket in the middle of each one. You can drill and screw through the waste first, but and I'll talk you through my approach on the large cutout as it worked quite well as an alternative. This is all to avoid those terrible tool witness marks from tabs.

1) Use an inside profile with a 1mm offset (remaining stock on the side wall) WITH TABS.


2) Then drill through the tabs with a cordless drill to remove the waste:


3) Manually jog the machine to remove most of the tabs (not critical to get all of it)


4) Clean up profile pass to remove the last 1mm. I do this in 2 stages as this is what works for my machine. 1st cleanup 3mm DOC, 0.9mm WOC, final cut full DOC, 0.1mm WOC.

Gives this surface finish:


Then bolting down, removing clamps, and onto the profile cut:


Same approach as above using a rough cut leaving 1mm stock, then semi-finish 3mm DOC, 0.9mm WOC, and finish full DOC, 0.1mm WOC. A stiffer/better machine might do the finish in one pass. I'm also limited to 6mm max cutter on ER11 collet. Good finish anyway:


Mirror part cut the same way, then some holes tapped and surface cleaned up:


The bearing end plates were done in the same way:


Then onto the bearing holders:




They will be a light press fit:


Second one made:


Trial fit onto the bearing plates:


This allows the ballscrew end bearing position to be fine tuned when setting up.
__________________

Moving away from the X axis and onto the Y axis - the belt tensioning system progresses. Turned some standoffs to hold the adjustable belt guide bearings:



______________________________

Looking ahead I need to turn down the end of one of the ballscrews. Made these 2 bits to hold it in the lathe. First is a protective collar to stop the jaws damaging the ballscrew:


Made it by boring a hole into some round stock on the lathe.
Then machined a hex onto some round stock:


Then used the hex to give 120 degree spacing to machine the 3 slots. Don't have a hex collet block which would have done the job!


Then back to the lathe to part it off:


Then to support the end of the ballscrew as it passed out of the headstock a spider/collar to fit inside the lathe spindle bore and hold the ballscrew. The ballnut is then 'tightened' up against it. Copied the whole idea off Youtube so should be OK!

[Chaz]

OK, more updates. To finish off the info on the bed rail supports, here is the little jig I made up to hold the bosses in place:


Here it is in position:


It uses 6mm shoulder bolts to give a good reference position and picks up off the inner tapped hole already there. This holds the boss in just the right place for welding. It's now ready for welding - just need to catch my friend with the welder in the next few days or so. This is bolt down the supported rail which obviously uses a pair of bolts on either side of the flange.
I've also taken the opportunity to spot out the holes for a profiled rail (i.e down the middle) to make a future upgrade much easier to do.


Next up are the end plates which hold the motor mounting plates. Starting with a nice skimmed off the sacrificial board:


Then setting up:

(note that I've scribbled down the X, Y, Z coord of the workoffset on the drawing - I always write them down in case of power failure)

I'm making a mirrored pair here. A few holes, and a large pocket in the middle of each one. You can drill and screw through the waste first, but and I'll talk you through my approach on the large cutout as it worked quite well as an alternative. This is all to avoid those terrible tool witness marks from tabs.

1) Use an inside profile with a 1mm offset (remaining stock on the side wall) WITH TABS.


2) Then drill through the tabs with a cordless drill to remove the waste:


3) Manually jog the machine to remove most of the tabs (not critical to get all of it)


4) Clean up profile pass to remove the last 1mm. I do this in 2 stages as this is what works for my machine. 1st cleanup 3mm DOC, 0.9mm WOC, final cut full DOC, 0.1mm WOC.

Gives this surface finish:


Then bolting down, removing clamps, and onto the profile cut:


Same approach as above using a rough cut leaving 1mm stock, then semi-finish 3mm DOC, 0.9mm WOC, and finish full DOC, 0.1mm WOC. A stiffer/better machine might do the finish in one pass. I'm also limited to 6mm max cutter on ER11 collet. Good finish anyway:


Mirror part cut the same way, then some holes tapped and surface cleaned up:


The bearing end plates were done in the same way:


Then onto the bearing holders:




They will be a light press fit:


Second one made:


Trial fit onto the bearing plates:


This allows the ballscrew end bearing position to be fine tuned when setting up.
__________________

Moving away from the X axis and onto the Y axis - the belt tensioning system progresses. Turned some standoffs to hold the adjustable belt guide bearings:



______________________________

Looking ahead I need to turn down the end of one of the ballscrews. Made these 2 bits to hold it in the lathe. First is a protective collar to stop the jaws damaging the ballscrew:


Made it by boring a hole into some round stock on the lathe.
Then machined a hex onto some round stock:


Then used the hex to give 120 degree spacing to machine the 3 slots. Don't have a hex collet block which would have done the job!


Then back to the lathe to part it off:


Then to support the end of the ballscrew as it passed out of the headstock a spider/collar to fit inside the lathe spindle bore and hold the ballscrew. The ballnut is then 'tightened' up against it. Copied the whole idea off Youtube so should be OK!

Very awesome, loving the work you are doing.

[JAZZCNC]

Coming along nice mate keep it rolling.

[Davek0974]

Some quality surface finishes there, nice :)

[Clive S]

Very nice build log I follow it very carefully its a credit to you. You could also call it tips and tricks

[routercnc]

Well, thank you all for the kind words of support. Means a lot, especially coming from the seasoned machinists on here.

I've re-read some of my latest posts and have realised that they paint a glowing picture where everything I do is perfect and works first time. This is misleading for the novices out there so I've decided to include things that went wrong for posts where there is something of interest. Readers have just as much to learn from things that work for me, as well as what not to do!

So here are some things that did not go so well / areas for improvement.

1. When making the bearing holder I'd broken my last good 6mm carbide the day before and a new one had not arrived. So I was stuck with an old blunt one. To give it a fighting chance at the pocket I chain cnc drilled out some of the material using a 3mm drill bit:


But the carbide bit made a nasty noise and was not happy. I switched over to a 3mm carbide and carefully cut it out. You can see the evidence of the 6mm blunt carbide on the top surface:


I had another look through my draws and found a single flute 6mm carbide which I've used for plastic. I cut the outer profile out with that one, plus all of the second part.

2. The 'second part' in the photo was actually the third part:

The real second part went on the scrap pile. On the drawing I'd called for a 36mm bore to take the bearing. After the roughing cut (~1.0mm under) I offered up the bearing and it almost fitted. Scratched my head and measured the bearing and it was actually 35mm. Using Vectric 2D you cannot leave stock etc so the quickest fix was to frig the tool diameter (e.g. telling the software that dia is '8mm' whereas it is actually 6mm gives you 1.0mm stock). Rather than re-draw the part, CAM, etc. I did a quick calc and frigged the tool. Bearing dropped in the new bore with 0.5mm clearance all round. Useless! Thought about making a sleeve, but 1.5 hours later had a replacement made with the proper size bore.

3. The radius on some of the corners is exactly 3mm. This is bad practice with a 6mm bit as there is suddenly a large tool engagement which leaves a witness mark. Better to go with 3.1 or 3.2 if radius is cosmetic. Look at the bottom right inner radius to see the slight chatter. Not a big deal, but one to be aware of.


4. Vectric cut 2D does not have lead in/out. This means there is a tool witness mark at the start / end of the finishing cut. You can help with a ramp in, but the exit goes straight up past the side of the work leaving a groove/scratch. Look at the wall near the top left screw:


Let me know if the bad stuff is as interesting as the good stuff and I'll include that too . . .