Sizing the starting blank

[Dave SParticipant @daves59043]

Wondering how people using CNCs go about the initial stock problem?

I have a part that’s pretty much 49x9x29mm (is not quite that simple, but for the sake of this it can be).

So I’ve done the CAD and the CAM and in the setup I make the initial block 50x10x30mm

All good, let’s go cut some metal…

I hacksaw out a piece to use, whack it in the big mill to square it up and make it to size. On measuring it ends up at 50.3×30.4×10

Do you:

A) go back and change the CAM,

B) machine the block a bit more, or

C) just ignore it?
Im leaning towards A as C feels risky – the initial cut is bigger than expected, and B could end up with undersized block. That’s less risky I think from the cut point of view, but more if the part now doesn’t fit.

Dave

[blowlampParticipant @blowlamp]

Does your CAM package take stock size into account?

Which CAM are you using?

 

Martin.

[FulmenParticipant @fulmen]

Just make the blank a tad bigger in the CAD model. You’ll cut some air, but that’s better than breaking taps.

[Dave SParticipant @daves59043]

I’m using Fusion 360.

The CAM setup starts with defining the blank, and in multiple setups the blank from the end of the last op becomes the starting point for the next.

Dave

[DC31kParticipant @dc31k]

I have just watched the latest HAL Heavy Duty YouTube video and he uses the wear offset of the tool to change what is cut from the stock.

Would it be correct that if you tell the CAM that the tool is larger, it will start further away from the 50mm defined stock and thus the first pass will not cut deeper than you wish it to?

Once the first pass has completed, you might need a nominal/virtual tool change to something that is defined as the correct diameter.

A future way of working might be to define the blank considerably bigger than it will ever be and just let the first few passes cut air.

[JasonBModerator @jasonb]

I usually make the blank a bit larger in setup, eg allow 2mm all round when I actually intend to use a piece that is approx 1mm bigger all round. This not only allows for the piece being a bit bigger but also less need to set it up spot on which can result in the first pass being deeper than you intended.

Alternative is to just go back and enter the actual (relative) stock size and regenerate the paths.

Just be careful what you use as a datum as a pair of edges is more likely to see a difference in cut depths on opposite sides than using the middle of the stock as your datum.

Size of cutter does come into it a bit too, assuming your 0.3mm over on length resulted in a cut 0.15mm deeper at each end than that is not really going to bother a 6mm dia cutter on an adaptive path but could have a lot more effect if you were going straight in with a 1mm cutter possibly doubling the DOC.

Some jobs can be better off doing a separate body to use as the stock, eg if it is an L shaped part on plan you could saw a lot of the waste material away rather than mill it. In which case sketch and extrude a body that is oversize but L shaped

[blowlampParticipant @blowlamp]

If you enter the actual stock size into Fusion 360 it should recalculate the toolpaths accordingly.

 

Martin.

[Julie AnnParticipant @julieann]

Not sure I have understood the issue, but I always use features on the part for aligning the CAM toolpaths rather than the stock? When generating CAM I add stock that replicates the overall dimensions of the part. The stock is only there to visualise the correct material removal and check tolerances.

There are two basic starting points. When the part itself is rectangular I mostly start with stock that is the correct size. I expect that general squaring up of stock on the manual mill will be within a thou or so of design size. For a part that has a non-rectangular profile I start with a rectangle that is a millimetre or two larger than the extremes of the part. On these of parts I pick up on a feature on the part such as a hole. The first operation will be profiling with multiple steps inwards so just add an extra step to the width of cut if needed. One will cut air for a period but for low part quantities it is not worthwhile spending hours fine tuning the CAM. Plus, when the CNC mill is running I can go and do something else.

As an example these parts started as a rectangular blocks of hot rolled steel to within a thou of final size:

The position of the two holes in the lugs are the only critical dimension; all three holes were drilled in the blanks on the manual mill before CNC machining. The reference point on the part for each operation was the north west point and top surface. This was set with reference to the fixed vice jaw and ‘zero’ height set from the work with tool 0 so that the tool height table entries were correct.

For these expansion links the positioning of the three holes are critical and they were drilled/reamed on the manual mill using the DRO. The outline is anything but rectangular so I used the middle hole as the zero reference:

The expansion links were mounted on a fixture with accurately drilled holes for bolts. Before CNC machining the oversize blank was mounted using bolts in the two outer holes and a co-axial indicator used to set zero to the middle hole. Then the third bolt was installed and CNC machining commenced:

Profile first followed by roughing out and finishing the curve slot. The slot was left a thou undersize to allow for hand fitting of the die block.

For odd shapes like the L mentioned I will start with a rectangle and a profiling cut so that the CNC mill generates the waste part. I wouldn’t spend time milling it all away.

Julie

[JasonBModerator @jasonb]

I don’t think there is any one right way that suits all, each individual part needs the approach that best suits it.

I’ve done parts that have no easily located feature so will allow the stock to be oversize and use it’s flat bottom as my height reference and the ctr of the stock for X&Y that way I know I will not have an uncut area on one edge and can set my tool heights when chaging tools.

Others which have holes in I may well use one of the holes as my datum, if drilled and reamed on the manual machine first or as a sseperate operation on the CNC I can then use those holes to hold the part. The the jig plate is drilled on teh CNC then the hole in the jig will be placed at a fixe dpoint so you don’t need to worry about locating it. Things like Conrods I do that way

Others I’ll use a body as the stock to more accurately represent what I’m starting with then the CNC won’t waste time cutting what is not there. This flywheel pattern for example was jig sawn to the pale transparennt yellow “stock” shape before going onto the CNC. Ctr of the flywheel used as datum and half cut at a time as I could not get it all in the Y axis

Another similar job the pattern was glued up from strips into a hollow box so my stock body had that same hole and foot material, sized as measured from the glue up. No need to use the CNC to cut out with a profile and leave a potentially loose piece of material to catch the cutter. Bottom of the MDF and ctr of the glued up blank used as datum.

 

[JasonB]

On JasonB Said:

I don’t think there is any one right way that suits all, each individual part needs the approach that best suits it.

That sums it up; horses for courses. It is also one reason that CNC milling is not the simple button pushing exercise claimed by the naysayers. With CNC you need to think ahead about reference points and how to hold the part, especially when multiple setups are needed.

I got fed up zeroing tools, and chipping edges on carbide cutters, at each tool change so I now use an automated electronic tool height setter to fill the tool table. I modified the postprocessor to implement a tool change including reading the appropriate tool length from the table.

Julie

[Dave SParticipant @daves59043]

Thinking ahead for multi setup operations is also needed in the manual world, it’s just that the CNC cans then go on and do a tool movement which is not generally possible with only 2 hands.
I’ve mostly been setting work zero to the front left corner for the initial blank setup, maybe I should try centralised.

making the cam blank bigger than my sloppy machining tolerances (I just milled to a scribe line by eye) is quite obvious now it’s been pointed out.

Dave

[blowlampParticipant @blowlamp]

Working to the centre is what I do when possible. I find it quite straightforward to locate the centre of the part’s bounding box to zero (origin) in the X,Y directions in CAD before exporting to CAM. It makes it simple to centralise the stock in the mill before setting the machine controller’s zero point.

 

Martin

[JasonBModerator @jasonb]

It probably also has something to do with the way you use a manual mill. I’m more likely to find ctr and work from there and that is how I dimension my drawings and the DRO is not bothered about backlash. However if you are more used to using the handwheel dials than the rear left corner is common as you then feed the handwheels in a positive direction. It also tends to mean you are using the fixed jaw as a reference as the back edge of the work is against that and should be more accurate for multiple parts than the moving front jaw.

Small parts I’ll often just cut from the next up nominal size round bar so set my datum as the ctr of the round bar placing the top of the work as the end of the bar unless it’s sawn in which case I’ll just use the jogs to mill it flat.

I also don’t scribe many lines, that bit of bar I would have taken a cut, measured with callipers and then cut off the difference to arrive at what I wanted.

If I used the CNC more than the current few hours a month then it might be worth getting say 10 or 12 holders and keeping the commonly used tools in those all with there lengths set but I’ll stick with what I use for now and put the pocket money towards metal for the next engine.

[Julie AnnParticipant @julieann]

Using the centre of a part for reference can be useful where mirror symmetry exists and/or when there is no point to pick up on the blank.

For these two name plates I wanted to CNC mill the outline, and pocket out the lettering, with seperate programs, and make two parts without moving the blank material:

Here is the fixture used:

There are two sets of 8BA holes, spaced 25mm apart in Y, for fixing the work down and one central hole to set X/Y zero. The Z zero is the fixture top surface. After picking up the zero positions a blank sheet of engraving brass was attached to the fixture with 8BA screws. The first outline was machined with a 3mm cutter, then the Y reference moved 25mm and the program run again. Then change to a 0.5mm cutter, move back 25mm and run the second program. Finally move the Y reference 25mm again and repeat.

Like Jason I rarely mark out for general machining, just use micrometers and the DRO. The only time I regularly mark out is when doing sheet metalwork.

Julie

[Author]

Posts