Here we go again . . . MK4

[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:
Attachment 20182

Here it is in position:
Attachment 20183

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:
Attachment 20184

Then setting up:
Attachment 20185
(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.
Attachment 20205

2) Then drill through the tabs with a cordless drill to remove the waste:
Attachment 20187

3) Manually jog the machine to remove most of the tabs (not critical to get all of it)
Attachment 20188

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:
Attachment 20189

Then bolting down, removing clamps, and onto the profile cut:
Attachment 20190

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:
Attachment 20191

Mirror part cut the same way, then some holes tapped and surface cleaned up:
Attachment 20192

The bearing end plates were done in the same way:
Attachment 20193

Then onto the bearing holders:
Attachment 20194

Attachment 20195

They will be a light press fit:
Attachment 20196

Second one made:
Attachment 20197

Trial fit onto the bearing plates:
Attachment 20198

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:
Attachment 20199

Attachment 20200
______________________________

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:
Attachment 20201

Made it by boring a hole into some round stock on the lathe.
Then machined a hex onto some round stock:
Attachment 20202

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!
Attachment 20208

Then back to the lathe to part it off:
Attachment 20203

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!
Attachment 20204

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 . . .

[njhussey]

It's all interesting!!!....good to see the good as well as the bad...if you want to see ugly ill show some of my stuff 😁

Sent from my HUAWEI VNS-L31 using Tapatalk

[AndyGuid]

It's all interesting!!!....good to see the good as well as the bad...

Ditto!
And this novice (little old me) finds your posts very easy and a real pleasure to follow.
Many Thanks, routercnc!

[routercnc]

Brief update. Next up were the plates which hold those bearing holders . . .

Setting it out, drilling out some of the holes and pockets:


Then bolting down through the holes so I can machine around the outside:


Quick trial fit to make sure all is well:


Went OK but broke a bit when I called for an 11 mm DOC instead of 1 mm in the CAM and didn't stop the machine in time.

I couldn't fit the standard ballscrew blocks in under the end of the gantry so am making my own. There will be 4 in total, 2 each side to allow me to pre-load one ballnut against the other to remove the 50 microns or so of ballscrew backlash. Here are 2 of the blocks, with 2 more on order:



I need to machine 45 degree chamfers on the top of the block but don't have an Engineer's vee block


So I machined up a jig with a 45 degree notch:


Here it is in position to show the idea (tabs yet to be filed off):


Then the blocks had to be squared up. There are lots of videos and info on how to do this on the internet so I won't repeat in detail. Great example here:
https://www.youtube.com/watch?v=tW8HNAlUXxU

In the photo below you can see a raw block (right) and the squared up block in the jaws (left). The brass rod is used whenever an un-machined face is against the clamping jaw otherwise it won't sit flat against the fixed jaw. The deadblow hammer is to make sure the part is seated in the vice.


Once squared up I set it up against a backstop (actually a parallel doubling up as a stop - must make something better !). It is now ready to have the details machined into the end such as the ballnut mounting holes. I can't machine the large clearance hole right through the centre because the part is 50 mm long. Even machining both sides its a bit too deep. So my plan is to bore a precise 20 diameter pocket in the end (say 10mm deep), then set it up on the 4-jaw, indicate on that bore to centre it, then bore it out.

[paulus.v]

Very nice build and documentation of the process. Thanks!

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:

You could split the finishing contour line and add radii in CAD if you are a perfectionist

[routercnc]

Very nice build and documentation of the process. Thanks!



You could split the finishing contour line and add radii in CAD if you are a perfectionist

Interesting thought Paulus. I see where you are coming from but would I end up with an open contour? I'll check it out but I think Cut2D only accepts closed contours. Longer term I'm transitioning to Fusion 360 where these more advanced options are standard practice.