CNC Router V1.0 (For Cutting Multiple Materials)

[biketrialsdave]

OK, so I warned of a whole heap of questions when I first started this project. Here are a few of the ones at the top of my list... If anyone would be kind enough to answer just one that would be very much appreciated! I hope they make sense...

1. Should I rebate/slot the aluminium plate where the aluminium extrusion butts up against it? Would there be anything to benefit alignment strength wise? I have done this with the extrusion piece connecting the gantry sides at the bottom but was thinking of the main X and Y extrusions.
2. This is a general tolerance question. Should I perform a worst-case tolerance stack-up when calculating tolerances for holes etc? A particular question I have regarding this is the diameter of the bolt holes. I want a close-fit to aid with alignment. EDIT: So for example an M8 bolt, what clearance should I include and what is a realistic tolerance if I have the aluminium plate machined manually or on a CNC mill? I'm going to use the ANSI dimensions for hole clearances etc. Should I go for close or normal fit for bolt clearance?
3. Following on from the above question...Another particular example of the tolerance question is where the Hiwin carriages are recessed into the gantry 'uprights'. The carriage blocks are 44mm high (I cannot see a tolerance in the datasheet...). Lets assume this tolerance is +/-0.1mm. Should I specify the slot in the upright to be 44.2mm +/-0.1mm? This would ensure the part would definitely fit, however if the carriage was only 39.9mm then this fit may not be tight?
4. Would my design benefit from an Aluminium plate across the back of the two extrusions on the X axis? If so, should I mount this to the two gantry 'uprights' as well as the extrusions? Would 10mm thickness suffice?
5. In my current design I have the Y axis hiwin carriages mounted to the lower portion of the 80x80 extrusion profiles. Would there be much difference/benefit in mounting these to the upper portion?
6. How do you determine how heigh to have your Z axis? What I mean by this is do you design around a typical flute length and add some? Should the Z axis be able to go through the bed?

Cheers,

Dave

[biketrialsdave]

Thank you very much! I will digest this information tomorrow...hopefully get let out of Jury Service early!

Dave

[biketrialsdave]

Little update... It doesnt look like much has changed but I've added a lot of minor details. Currently ALL aluminium plate is 20mm thick. Does anyone think this is overkill for the plate which attaches to the X axis carriages (on top of gantry) and the plate which attaches the motor mount to the Z axis?

My useable bed dimension is now 343mm x 434mm. I think that's fairly reasonable for what I will be cutting.




Dave

[JAZZCNC]

If I have read this correct, the top edge "registers" with the carriage (i.e. points it in the right direction?) but does not actually have a close/touch fit with the carriage?

Yes the top edge sits directly on the carriages, the edge acts has the register. If you have them already look at the carriages and at least one edge will be machined, this the the reference edge.
The rails will also have a Machined Ref edge, exactly the same applies with the rails regards Referencing against an edge thou in your case using profile you will only be able to do this if you machine the profile or have a separate plate machined which bolts to the profile.

Another question regarding clearances... I am in the process of adding milled out sections in the end plates to locate the extrusions. Should I allow an additional margin (say 0.5mm??) for the extrusion? Or should I design an 80x80 slot with 4mm radius corners as per the extrusion?

The only sure way is to measure the profile your using then machine to light interference fit. Wouldn't suggest you have them machined without the profile first if your wanting close fit.
Same goes for anything you want machined really, don't trust Cad or dimensional drawings where fit is important has there is always some slight difference waiting to bite you. Can't beat having the part in your hands and I won't machine anything were tight or close tolerance is important without parts in hand.

Currently ALL aluminium plate is 20mm thick. Does anyone think this is overkill for the plate which attaches to the X axis carriages (on top of gantry) and the plate which attaches the motor mount to the Z axis?

Nope it's perfect and will help reduce resonance. . . .Certainly wouldn't go below 15-16mm.

Can I suggest you change the position of the BK/BF bearing blocks and put them on the outsides of the gantry and End plates, or at least the motor side bearing.?
The way you have them on the inside will mean they are trapped between the gantry side and end plates which will make fitting very awkward and inflexible, will also mean they need to be done at the same time has bolting profile together.

Put them on the outside at the motor end and you can insert the screw thru the ends/sides after building frame. Notice you have the motor mounts has closed blocks like this so just machine the inside to clear the bearing block and fitting will be much easier and very neat, The bearing will also be protected from crap inside the motor mount so that's another plus.!!

[biketrialsdave]

Quick question, do end mills tend to come in 'standard' lengths? I am still struggling to calculate my Z axis height. I only have 90mm of travel to play with on the KR33 so it's fairly critical.

On a side note, I have fairly drastically reduced the size of the plate which attaches the motor mount to the KR33. The idea being that the motor mount is almost exactly centralised on the two KR33 carriages to reduce canter-levering effects. Good idea?


Dave

[JAZZCNC]

BUMP BUMP.!!

Thought I'd replyed to this question.?? Obviously not but did mean too.!


Look more towards drills has they tend to be the longest things you'll put in the spindle.
Endmills can be various lengths depending on flute length. Common 6mm typical standard endmill will have a flute length around 12-15mm and stick out around 18-20mm. Overall length roughly 55mm.

[biketrialsdave]

Thanks JAZZ, I will do some calculations.

There is one thing that has been bugging me for a long time regarding setting up material to be cut. Here goes!....

1. Lets say I have placed an aluminium billet roughly in the centre of my bed and I want to cut a simple motor mount out of it. Lets assume that the billet is slightly bigger than the size of the motor mount. How do I align the router up so that the flute is in the right place to start cutting?! I assume that if the billet is larger than the part then you would manually put it in the corner somewhere?

2. Now here comes the real question. Lets assume I have finished milling one side of the mount and I need to turn it over and mill the other side. How do I ensure that the mount is in exactly the same place once flipped?! Or would you put it in a new position and somewhere align the cutter in exactly the right place to start cutting?



I hope I am not missing something obvious here! :)

Cheers,

Dave

[biketrialsdave]

Bump

[m_c]

1. if the billet is oversize, just touch of roughly from the relevant sides. Touching of can be as simple as with the cutter spinning, just jogging up until the cutter marks the material, then hitting the relevant zero button (or entering size if not working of zero)

2. Depends on tools at hand, and how many you'll be doing.
For any more than a few, you really need to make up some kind of jig capable of accurate mounting.
However for one offs, you really need some kind of additional tool. For cnc, a touch probe is the best suited, however there's nothing stopping you from using old manual techniques, such as edgefinders, dial gauges, bit of paper stuck on, and jogging up to where you need to be.

[JAZZCNC]

M_C answered most of it but here's couple more suggestions.

1. A: Good Habbit to get into starts at the Cad when you define the part. I always place it 2 or 3mm in from X0Y0 then when you touch off the billet side you know you'll always be inside it and won't run off the edge.
B:Another way is to draw the outline of the billet in cad and have X0Y0 on the corner and work piece inside it.

2. Easy way for one-off's if working from square/rectangular billet is to use the billet corner has X0Y0 like in option B: above then when you flip just make sure the edge is parallel to Axis and pick up X0Y0 from corner again.
Problem comes when you can't work from square/rec stock or if need to relocate already completely machined parts.?
In this case then it's often better to place X0 Y0 in cad on a hole centre or other defining feature that's easily picked up off using touch probe or other manual technique.

Regards the touch probe then doesn't need to be any fancy or expensive tool just piece of wire with plate on the end of a known thickness and using a spare input setup in the control has probe input. Then put plate between tool and work piece.
So long has the tool diameter is known you can just use what ever tool is in the spindle for quick touch off, if you want very accurate position then best to use accurately known shaft or tool shank.
(Tip: If your working with Ali or metals and can isolate the work piece from the main frame or Ground then you don't even need to put the plate between the tool and work piece so can enter just tool radius into DRO for offset. Just touch probe wire to work piece.)

This can then be used in few ways either by using the G31 probe command directly and telling it the axis direction and distance to travel looking for the edge.
Then when it's touched off you zero the Axis DRO's and type the radius of the cutter + plate thickness directly into the Axis DRO to give correct offset from edge.

To find hole centres you'd do this for each X,Y axis if you know the hole radius then type that minus the cutter radius + plate thickness has either positive or negative value depending on which side of hole you probed has the new offset.

With that said the best way and easiest way when it comes to probing is to use pre designed scripts with probe commands etc for each type of probe routine you want to do which does all the offsets etc for you then add a button to your screen set so it's a one click affair.! . . . OR . . .
By far the best and easier way if you use Mach3 is just buy Gerry's 2010 screen set which has all the probe routines you'll need and more besides. The CNC Woodworker - Mach3 2010
With this screen set and simple touch plate on wire you'll very accurately find most locations and will be the best £15 you ever spent.