Dan Heeks's Milling

Engraving Aluminium Alloy

2012-01-30T23:58:00.000Z

I sharpened an engraving cutter to a finer point, approximately 55 degrees included angle, instead of 90 degrees, with a clearance of 1/4 of a thousandth of an inch per 20 degrees rotation of the tool, with an initial clearance angle of about 13 degrees ( I hope I remember what I mean by all these numbers, so I can do it again ). The flat of the cutter was no more than 0.1mm diameter, which is dangerously fine. The material was aluminium alloy. Cutting time about 10 hours. 50mm/minute horizontal feedrate. 20mm/min vertical feedrate. The result was beautiful. I can't wait to see the impression it makes. I hope it doesn't get damaged in use too quickly, as it's not as hard as steel. Interesting marks on the surface must be because of a lack of coolant; I couldn't stand there for 10 hours, so I just put some oily paraffin on the surface, but I guess it got used up or dried out while I was out at work.

Hardened Steel

2012-01-20T22:34:00.000Z

Bad news: Broke a cutter.
Good news: Found dad's packet of 90 degree engraving cutters
Bad news: Kept breaking them until I only had two left
Good news: Discovered that the steel I am using is much harder than some of the other steel I got.
Bad news: I want to wait for this one to be finished, but it's cold in the workshop
Good news: I have a small office and a fan heater, so I'll be warm in no time

The cutter broke to some extent on the first couple of passes on all of the above attempts and got steadily worse from right to left.

Roller-pressing onto copper

2012-01-19T10:34:00.000Z

We have put the steel with ridges through the roller-press with some copper. It actually looks ok in most places. We need to modify the design though to make sure there are no areas with lines running nearly parallel too close to each other.

Engraving Ridges

2012-01-19T08:15:00.000Z

It took almost 10 hours to machine this; 21:30 to 07:30. I was using a fairly slow feedrate; 60mm/min, 5000rpm.
But we can see a problem where lines cross each other or get close to each other, the cutter can't get into the gap, because of the size of the flat.
Maybe we could use chemical etching to make this?

Toolpath for engraving ridges

2012-01-17T18:59:00.000Z

Instead of engraving grooves we wanted to engrave ridges!
I found this simple way to create the toolpath with HeeksCNC.
I drew all the ridges as sketches, made from lines.
I extruded the sketches down, 1mm.
I made a 3D attach operation and a zigzag pocket operation, specifying an engraving tool.

Tidier

2012-01-17T18:21:00.000Z

Almost finished tidying the workshop.

Rotary Axis

2011-11-23T11:03:00.000Z

I used my new rotary axis for my Sieg KX1 to cut a big gear ( 60 teeth, 77.5mm outside diamter ). Each side of the tooth is made with about 10 cuts, so it has many straight lines. It doesn't seem to run as smoothly as the gear which I milled around the profile.

Bridgeport Repaired. Auto Spindle Off added.

2011-11-20T13:32:00.000Z

I have spent 2 days fixing my milling machine.
The PC that I used to control it stopped working; the floppy drive had failed and none of my 6 spare floppy drives worked, so I guss it was a motherboard problem.
I found another old PC to run the software on. Fortunately, I found the source code for my PC control ( "Heeksatrol" ) which I wrote in about 2001. So I was able to modify it.

I took the opportunity to automatically turn off the spindle when the tool needed changing, or the program had finished running.
I looked at the relays and tranformers in the machine, but decided to simply add a RC servo to physically turn the spindle switch. I made my program output on one of the unused parallel port pins and connected an Arduino with the servo attached ( source code here ).

While calibrating the speeds, I blew some of the machine's power transistors, so I had to replace them.
Anyway, now my machine cuts metal and turns the spindle off, so I know when to jump up and change the tool. :)

16mm needs sharpening

2011-10-21T20:00:00.000+01:00

Listen to this cutting. Do you think I need a sharper tool? :)
It's a 16mm diameter HSS milling cutter.

milling gears

2011-08-12T18:03:00.000+01:00

I can make module 1 gears from acetal on my milling machine, using a 1mm diameter slot drill, for the teeth. I used a 6mm to rough it out and a 3mm slot drill to cut out the 4mm hole.

gears

2011-08-12T16:39:00.000+01:00

I made some gears and a casing, as an experiment.
Parts were coming out lozenged, but I fixed that by pushing on the table until something bent, so the axes are more perpendicular to each other. I tested this by checking the nozzle distance from the table at each of the corners of travel.
I was pleased with the gears I made. I ran them in a little with some brasso to get them free running.

pp3dp

2011-08-09T21:41:00.000+01:00

This is not milling, I know, but...
I bought a 3D printer from here http://www.coolcomponents.co.uk/catalog/product_info.php?cPath=89&products_id=644
It arrived this afternoon and I assembled it and got it to work, kind of.
The parts come unstuck while being made, which cause them to warp a bit.
Apparently I can fix this by sticking some Scotch Blue Painter's Tape to the machine bed, instead of using the green paint, they supply.
I don't know if I can buy any of this tape in Malvern, England.

I coloured the heart with a permanent marker. You can use solvent based paint for painting ABS, though.
The heart was almost 1mm undersize in both axes.

I liked the sound the plastic part makes when I drop it onto the table.

Making for money

2011-08-04T17:58:00.000+01:00

I have been doing quite a bit of machining work recently.

Clamping with one screw in the middle

2011-07-08T18:56:00.000+01:00

I am fitting a spur gear to a bigger spur gear by cutting an external hexagon, with small radiuses, on the outside of the gear's boss. Most of the work here was in cutting the right shape in the black acetal, including drilling and tapping a hole. The tapping was done by hand, with a tap in a chuck.

Gears

2011-06-13T10:07:00.000+01:00

I have started adding gear design to HeeksCAD. I am hoping to design some 3D models of bevel gears, but I have started with spur gears. Bevel gears are a bit complicated.

Engraving for jewellery rolling mill

2011-05-25T12:20:00.000+01:00

My girlfriend told me about how they put their silver through a rolling press with various items, at her jewellery class. So, I face machined a piece of 1.5mm steel sheet and engraved some mirrored designs on it. She took it to her jewellery class with some soft aluminium that I gave her and put them though the rolling mill. In the picture is the aluminium with the pattern pressed on to it. I think most of the pattern was too deep and has rough edges, but the shallower hexagon patterns were better.
The steel comes out bent, but you can use it many times.

punch for silver jewellery

2011-05-05T17:21:00.000+01:00

I made this punch from stainless steel for using on silver sheet for jewellery.
The photo shows its effect on pure aluminium.
I made it simply using a pocket and profile operation with HeeksCNC software on my Sieg KX1 milling machine. The design given to me was pencil on paper. I have noticed that the result is the mirror image of the design. I hope she doesn't mind! I can easily make another one the right way round.

6 fins

2011-04-20T10:54:00.000+01:00

I did 4 in one day. Now I have to set up to machine the big hole.

Fin made from Acetal-C

2011-04-12T08:51:00.000+01:00

I am making 6 of these. It took me a whole day just to make 2.
The operations are:
* 16mm face machining leaving 4mm thick 8mm wide sections to fit into table - 10 mins
* 6mm slot drill - 15 mins
* 6mm ball nosed - 30 mins
* 6mm slot drill - 15 mins
* 6mm ball nosed - 30 mins
* 3mm slot drill - 0.3 mins
The rest of the time is tool changing and preparation. I think I might be able to make 4 in one day.

Hole down centre

2011-04-01T18:09:00.000+01:00

3D milling on both sides

2011-04-01T09:05:00.000+01:00

VoxelCut

2011-03-31T15:37:00.000+01:00

I have developed VoxelCut a bit more, so I can test my machining toolpath.

3D milling

2011-03-30T18:12:00.000+01:00

I am using HeeksCNC to calculate toolpath for milling a fin for a robot submarine.
My first tests are in wood, using a 6mm slot drill and a 6mm ball-nosed tool.

I need to use a bigger piece of wood and machine a flat face and some dowel holes for turning the part over and locating it.

Dad's Machine

2011-03-05T12:55:00.000Z

Dad has fallen over and cracked a rib or two, so I am working his machine to get his work done for him.

It is a Bridgeport Series I with a Heeksatrol control. ( Heeksatrol is a PC with some software I wrote in 2001, inputting and outputting via the parallel port ).

Drag knife compensation

2011-01-25T11:22:00.000Z

Someone asked about calculating a path for drag knife compensation, so I had a go at writing an OffsetForward method for my Curve class. See the code here.

Part 0018

2011-01-15T00:38:00.002Z

Part 0015

2011-01-14T20:14:00.000Z

Part 0014

2011-01-08T17:34:00.000Z

One of these flutes was still very sharp, so it should cut ok.

I did all the CNC work from one side, cutting small, 2mm deep, pilot holes, with a 3mm diameter slot drill, where the 5.5mm holes need to be. Clearing all the metal with the 6mm slot drill took 2 hours.

I cut the holes to 5.5mm afterwards on Dad's pillar drill.

For the counterbores, I countersunk them, on the pillar drill, oversize, then did the counterbore with a 10mm endmill.

There was only just enough room to cut the 2mm slot, but there was enough room, see video.

HeeksPython adding python interface

2010-12-26T12:52:00.000Z

HeeksPython now calls autoexec.py on start up, which can add menus and windows to HeeksCAD.

end holes

2010-11-26T17:34:00.000Z

These parts are too long to CNC drill the end holes, so I had to make a drilling guide first.
I used a 3mm milling cutter to pocket and profile the shape in the Delrin, then I used the pillar drill and put the aluminium part in the portable vice and held the Delrin guide onto the end of the part to do the drilling. I only used the guide to drill a small depth, then I drilled them through later.

Ungluing accident.

2010-11-03T20:24:00.000Z

See my coolant delivery system in action in the video.

I had a problem with this part. The sawn piece was a tight fit in the pocket in the wood sub-table, so it didn't glue well, so it came unstuck soon after the start of machining. You can see the bent path left in the metal, in the video. I remachined the wood and chiselled the side of the pocket bigger and everything else went well, but there is a bit of a gouge out of the top of the circular post feature. Maybe it won't matter too much? The surface finish doesn't seem any different ( the one on the left of the picture is the most recent part ), despite lowering the feedrate to 50 mm/min instead of 100 mm/min. The tool looked slightly worn after the ungluing accident. It doesn't look much more worn after all the machining, so I think that 200 mm/min is better than 300 mm/min. Hopefully the next one I make won't have any mistakes in it.

Part 0012, number 2

2010-11-03T12:26:00.000Z

I have made another of these parts. This time I tried 3mm depth of cut. It was OK. Also I tried using climb milling for the finishing pass, instead of conventional milling. It isn't much different. Also I put the coolant guard back on, so I could pour the coolant on quicker. I made a mistake with the program for this one and there is a gouge, see the second picture. The tool is very battered. It has only made 2 parts. I noticed it was a bit damaged after the first part, but it is a lot more damaged now. I will try reducing the feedrate from 300 to 200. I will use a new cutter now. Also, the later roughing cuts are leaving the material up to 0.1 too thick. I can't explain this yet, so I will try it again to see if it happens again.

Part 0012 without holes

2010-11-02T00:06:00.000Z

I made this part. No holes in the ends yet, though. The surface finish could be better. I am doing the finishing pass at a feedrate of 100. Maybe I should try 50?

Most of the time was spent doing the roughing, because I was only happy descending 1mm at a time with the 6mm tool. It took about 2 hours machining.

Part 0012, Roughing

2010-11-01T13:12:00.000Z

The next thing is to calculate roughing toolpath. Here I have made the flat faces into sketches. I have had to draw some extra sketches. If the sketches touch each other, HeeksCNC joins them together nicely. I had to enter the z values correctly. Maybe one day I will automate all of this. There are 6 separate pocket operations.

Part 0012

2010-11-01T12:17:00.000Z

I am going to make this part out of aluminium alloy.

The first thing is to saw out a piece of Delrin as the sub table and pocket a shape oversize, for the aluminium rectangle to fit in. I can specify to cut a sketch oversize by putting a negative value in the "material allowance" box. I am using a development version of HeeksCNC, which includes a commercial pocketing library written by Lou Lavery, that I am planning on reselling as an option for HeeksCNC when it is ready. I am trying to write a free version of pocketing, but it's not easy.

Pocketing Reorder

2010-10-21T15:10:00.000+01:00

Now, in HeeksCNC, you don't have to worry about which direction ( clockwise or anti-clockwise ) your sketches are drawn. Simply select them all, do "Combine Sketches", then select that resultant sketch before making a pocket operation. The python script now uses the new function area.Reorder(), which checks which curves are inside which and reorders their direction ready for offsetting.

Commercial Pocketing Software

2010-10-15T18:11:00.000+01:00

I have been asked to help someone make a commercial Windows dll to do pocketing like in HeeksCNC. Unfortunately the polygon offsetting used in HeeksCNC is derived from the "kbool" software, with its' GPL license, so it has to stay free. I have done quite a lot of work recently to adapt the "Clipper" polygon clipping library to do offsetting too.

Here are my results.
The first picture was made using kbool.

The second picture was made using my modified version of clipper.

More dialog work

2010-09-30T22:29:00.000+01:00

I tidied up the pocket dialog.

I noticed that if the viewing units are in mm, but the NC output units are inches, then all the values in the dialog are in mm ( which is what I expected ) except for the tool description. I am reluctant to change it because the tool decription is used in the comment in the NC code comments, so maybe it should be in NC code units for that.

Pocket operation now uses a dialog

2010-09-23T23:02:00.000+01:00

I have added a pocket operation dialog. When you select a sketch and add a new pocket operation, you get this dialog. When you OK it, the pocket operation gets added. When you double click the operation in the tree, you get the dialog again. When you select a different control, or press Tab to go to the next control, a different picture is shown.

opencamlib operations working again in HeeksCNC

2010-09-23T22:01:00.000+01:00

The 3D operations weren't working in HeeksCNC because of some changes that had happened to the syntax in opencamlib . They work OK now. Here is an "attach operation" modifying the toolpath of a pocket operation.

zig zag option for pocket operation

2010-09-11T17:08:00.004+01:00

I added a "use zig zag" check box to the pocket operation in HeeksCNC. It seems to work really well. It works by making a rectangle for each slice of the area. It does a boolean "intersect" of the rectangle with the area to pocket. Then it loops through the resulting spans. It starts with the straight line at the bottom of the result and adds all the spans until it gets to the top of the slice. I also added a "zig angle" value too.

Keep tool down

2010-07-27T18:22:00.003+01:00

I changed the pocket operation to keep the tool down whenever possible.
I have changed the "area" module to make Subtract work again.
This is my function in area_funcs.py

def feed_possible(p0, p1):
....obround = make_obround(p0, p1, first_offset_for_pocket)
....a = area.Area(area_for_pocket)
....obround.Subtract(a)
....if obround.num_curves() > 0:
........return False
....return True

P.S. how do I get the spaces to stay at the start of the line in blogger?

Attach operation

2010-07-09T23:16:00.003+01:00

I have added an "Attach" operation.
You select a solid before making it.
Any other operation done, after an attach operation, will have its feed moves dropped down on to the solid ( or solids ) specified by the attach operation. This can be cancelled by an "Unattach" operation.
In the picture, an existing "Pocket" operation is attached to the cone.
This is not finished yet. I need to add a "minimum z" value to the attach operation; currently it is set to 0. Also, I need to decide if the z height specified in the existing operation should be taken into account. For example, if the pocket operation is trying to cut to z-1, should I make this be 1mm below the surface contact point?

End Plate

2010-06-20T15:20:00.004+01:00

I made another part from aluminium alloy.
There were a few lessons learnt here. The most exciting one was where I hadn't tightened the 16mm tool holder into its collet enough. I noticed the tool was cutting deeper than it should, so I paused the machine and set the z lower so it would cut higher.
I started again but it continued to cut deeper as it went. I stopped and adjusted the z value again. I assumend that something was going wrong with the Z axis drive of my machine. I continued to cut until the tool holder fell out and wedged over at an angle!
Fortunately nothing had been damaged, as far as I can tell, and the part had been cut oversize, where it went wrong, so it should be OK.
I had to stop there, yesterday. I came back this morning and tried again. I looked at various positions of the part on the computer and then set the x, y, z of the machine by touching the tool against already machined faces of the part, with a piece of paper. However, as soon as the tool started cutting metal again, the part came unglued. The coolant had unstuck the super-glue, overnight.
I pressed the big red button, took the part off, cleaned it up, machined a new area in the wood, with some islands to locate the part. It was a bit of a tight fit, so I hammered the part down to glue it down. This probably isn't good for my machine, although it is resting on a lump of wood.
I am happy with the finished part. I did have to hammer it straight again afterwards though.
Another thing, I have seen before, is where I am cutting a sharp inside corner ( or one the same radius as the tool radius ). On the finish pass, the amount of material taken off is quite accurate because there is not much deflection or vibration until it gets to the sharp corner. It then momentarily squeals as it cuts the entire corner in one instant. You can see from the last picture how there is a lot of deflection ( I gues about 0.3mm on my 6mm tool. A solution would be to change the shape of the pocket so that the internal radiuses are at least a bit more than the tool radius, or to use a smaller tool.

More Delrin parts

2010-06-15T20:13:00.004+01:00

Some more parts were asked for, yesterday evening. I have made them and will go to the Post Office tomorrow morning and send them first class.
I made the round ones first. My 6mm tool is cutting slightly too much material, so I set its diameter to 6.05mm for the other parts.

An aluminium part

2010-06-13T20:49:00.003+01:00

Yesterday, after drilling the holes for Part 0009 and making a couple of other small Delrin parts, I made this aluminum ( HE30 ) part for my friend Maaten. There was a mistake on the other side where a profile offset, for a counterbore, failed on HeeksCNC and I didn't realize. This caused the roughing passes to only have lead on and lead off moves, but no profile. The finishing pass, at full depth of 6.5mm was calculated OK, so when it machined the finishing pass, it was almost too much for it and the circular hole wasn't very round.
On the side we can see in the picture, the slots were mostly too wide, because the rough pocketing ( done with 0.1mm extra clearance at the sides ) was done in a "conventional" style, where the path goes clockwise, which caused it to take off too much material. I need to be able to specify "climb" or "conventional" for pocketing aswell as profiling.

Part 0009 done

2010-06-12T08:53:00.002+01:00

I have done these. There were 8 of them to make. My Z travel was not enough to drill them with the drill, which needed an extra chuck, so I drilled them to 3mm deep with my little slot drill, which fitted in the collet, and then drilled them through on Dad's pillar drill.
This is all of the Delrin parts done, for this customer.

Mach 2010

2010-06-11T14:37:00.002+01:00

I am here at Mach 2010, telling people about HeeksCNC software. I was thinking that Machine Tool manufacturers might be interested, but they mostly already have ties to commercial CAD/CAM software vendors. I spoke to Ian Walton from Cranfield University. I might help him make some software for his welding machine.

Parts 0010 and 0011

2010-06-09T16:17:00.003+01:00

2 of each. 0011 was similar to 0010, so I only had to write a couple of operations again.

Part 0010

2010-06-08T14:49:00.005+01:00

This part requires cutting on almost every side. The way the depth of cut works for pocketing is different to profiling in HeeksCNC. I must make them work the same.
For example the profile operation would have done this with depths of cut ( 5.125, 5.125, 5.125, 5.125 ), but the pocket operation used depths ( 5, 5, 5, 5, 0.5 )

Part 0007 finished

2010-06-04T20:37:00.002+01:00

I have made the other copy of this part.
I think there are issues with hole depths, because I made this part 10.3mm thick ( to be sanded down to size ), but then I assumed that that it was 10mm thick for some of the holes.
This should mean that some of the holes are 0.2mm to 0.3mm too shallow.
I'll come back and have a look at these later.

Part 0007 1 done

2010-06-04T12:00:00.005+01:00

I finished one of these parts. Now I must make another one. There are various things I am not happy about with this one. Having to cut it in at least 4 different setups has made it difficult to plan the clamping. In the top picture, I have cut the wood so that there is a post for one of the holes at the top right and an island for most of the big circle hole. This was not clamped ideally and you can see in the 3rd picture how the profile doesn't match up.
In the 4th picture, you can see where I made a programming error for one of the holes ( I had to program it separately from the others because of some geometry error I don't understand yet ). I accidentally typed the final depth in to the rapid-to height. This highlights the need for my software to warn me if the rapid-to height is below the start depth. In my next version of the software, the rapid-to height will be a relative distance above, instead of an absolute z height.

Part 0007 continues

2010-05-26T21:53:00.004+01:00

To get this far, I have written 14 NC files. They are:
001 6mm one quarter face milling
002 6mm counterbores
003 6mm big hole
004 3mm small holes
101 6mm wood area
102 6mm rectangle hole
102b 6mm wood area with island
103 6mm outside profile
104 3mm holes
201 6mm wood area
202 6mm right holes
203 6mm top right profile
204 6mm bottom right profile
205 6mm sub table

No super glue was used. I used double sided carpet tape for the facing operations.
I am using an adjustable spanner each time I change tool, because I don't have a 15mm spanner.
I don't have any safety spectacles.
Today I ordered both these things online as a reward for my hard work.

Part 0007 toolpath

2010-05-26T13:01:00.003+01:00

Sitting here waiting for this to be cut on the machine next door. I thought I'd show you the toolpath generated by HeeksCNC 0.13.0 on Windows Vista.
Click on the picture to see it full size.

Part 0007 - wood screw

2010-05-26T12:34:00.002+01:00

Here I am clamping by screwing into the wood. I drilled a pilot hole for the wood screw with a hand-held electric drill. I tightened the wood screw until I could hear the wood cracking.
But still I was not clamped tightly enough. In the picture you can see that the tool path has veered to the left as the Delrin has been forced to the right. Fortunately the part is not scrap.
I will re-cut the wood area with an island for the rectangular hole to sit in and try again.

Part 0007

2010-05-25T13:11:00.002+01:00

Part 0007 is a bigger job than I first thought. I had not noticed that the middle part of it is bigger in Y than my machine can handle. I will need to tackle it in many separate operations. The first job is to face mill it to the right thickness. I have programmed a pocketing operation to do a bit more than a quarter of it. I am using carpet tape to stick it down to the metal of the machine table.

Part 0008 finished

2010-05-21T22:56:00.004+01:00

What happened to Part 0007? Apparently it needs another hole in it, so I am waiting for the new CAD file before I start.
Part 0008 was interesting, because it introduced me to the vice and therefore the dial indicator.
The old dial indicator that dad gave me needed moving a few times before it loosened up and would spring back by itself. It is marked in increments of 0.001 inches.

Part 0006 finished

2010-05-19T15:14:00.004+01:00

I made these two.
This concave corner was drawn as a perfect corner. I have made it with a 3mm radius. I hope this is OK. Also the internal corners I made with a 3mm radius instead of the 2mm radius they were drawn with, so I could use my favourite 6mm slot cutter.
I am not so happy with the holes at the end. I machined a piece of wood with a hole in, as a guide piece to fit the end, then I drilled them on dad's pillar drill. The depth is pretty accurate, but the position is not good. If X is the 100mm side and Y is the 10mm side, then the position is accurate to X 0.02 on each of them, which I am happy with. But on one of them the Y is 0.20 wrong and on the second one Y is 0.10 wrong. For the second one, I put a clamp across the wood, which seems to have helped. I believe I need to use a better material as the guide. I should use an off-cut of delrin. The holes were drawn 6.4mm diameter. I used a 6mm drill and the hole ended up about 5.9mm diameter. I don't have a 6.5mm drill. I will buy a box of drills which include a 6.5mm drill and redrill them with a delrin guide, later.

Part 006 one almost finished

2010-05-18T15:28:00.007+01:00

This one is done, except for a hole in the end facing us. I need another one like this, though.

Part 0006 started

2010-05-17T18:47:00.004+01:00

This part will require machining in two different setups. First I machined some counter-bored holes in a piece of wood ( using the Profile operation ) and finished them with Dad's pillar drill. I bolted this on to the table using the t-slots. I machined an area flat on the wood. I super-glued the Delrin to the wood. I am doing some profile operations with 6mm slot cutter. Unfortunately I forgot to check that the Y-axis had enough travel in the position I placed it. It hit the limit while rapiding to the outside profile. The part is not scrap. I will need to do it again, but machine an area in the wood with an island left standing in the middle to locate the part.

Part 0005 done

2010-05-17T12:11:00.004+01:00

Dialog pictures

2010-05-15T23:18:00.002+01:00

I extended the properties window to be able to have a different window. This can be in addition to or instead of the property grid. My example for cuboid just makes a window with a picture, but I hope to make some windows with controls ( edits, radio buttons, pictures, list boxes ).

Part 0005 first side OK

2010-05-13T18:25:00.004+01:00

This works well. It is a bit labourious having to saw away all the wood, so it is flexible enough to peel off the Delrin, but worth it. Leaving 0.1mm on the depth is always a good idea. It doesn't take long to sand it to exactly the depth I want.

Part 0005 super glue

2010-05-13T16:58:00.003+01:00

I think carpet tape would be too inaccurate. Also I don't have any.
Super glue seems to stick Delrin to the wood strongly enough. Also, I can remove the piece from the wood with my pen-knife. Now, can I remove the super glue with hot soapy water and a sponge?...

Leaving it to soak in the washing up bowl...

No. But I can sand it off and nobody needs to know it was there. I'll leave a little bit extra on the face machining depth, so I can sand it down to the required thickness anyway.

Part 0005 attempt

2010-05-13T15:26:00.008+01:00

A daring attempt to not waste material. I wanted to do this one without needing tags.
It seems to go wrong on the above picture, where the two clamps can't stop the top edge lifting up a bit.The underneath of the arch seems to join perfectly, so the lifting edge went back to where it was when I moved the clamps. I might try clampless machining. If super glue works well enough, it might be worth clamping the Delring to the wood with super glue.

Part 0004 finished

2010-05-13T12:11:00.000+01:00

I made 2 more of these yesterday afternoon and I made 3 more of them this morning, so that is the 6 required.
With my method of clamping on to a sacrificial piece of hardwood, there are inaccuracies in thickness of the parts. If I clamp tighter, I get a thicker piece. Most of these pieces are between 9.96mm and 10.02 at the edges and about 9.85 to 9.95 near the middle ( depending which part you measure ), because of the way the piece is bending when clamped. But one part is about 9.88 all over, where I didn't clamp it so hard ( to try to reduce bending ). I could improve this, by using some aluminium to act as the sub-table, but this would make everything more expensive. I think these are meant to be fairly low cost parts. I will try clamping more gently for the facing operation, but adding 0.1mm to the programmed depth.

Part 0004

2010-05-11T16:30:00.000+01:00

I made Part 0004 correct, first time. There are 6 in total wanted of these. I got the chamfer to within 0.1mm of what I wanted, I think; it's hard to measure the chamfer. The subsequent copies should be more relaxing to make. There are no tags on this part. I cut the outside profile in two separate operations, so I could remove two of my four clamps and replace them to get to every part of the profile. I put my fingers on the part as it was being cut to catch the piece of scrap that falls off and to damp vibrations.

Part 0003

2010-05-11T10:51:00.000+01:00

I made Part 0003 correct, first time. I was able to re-use some of the operations from Part 0002.

This video shows the rough profile pass for the outside shape, done in two steps of 5mm.

Part 0002 finished

2010-05-10T16:40:00.000+01:00

I did Part 0002 again with no mistakes.
The chamfer is about 0.2mm under size. I don't think this will be a problem.

Part 0002 again

2010-05-06T16:33:00.000+01:00

Only one mistake, this time. The chamfer was too big. I worked out what I did wrong. I wanted to offset the path 1mm from the part, so I told the software it was using a 1mm slot drill. I should have told it it was a 2mm slot drill. The chamfer is 3.8mm instead of 3mm. I left on 0.2mm for safety, but it was not enough.

Part 0002

2010-05-06T10:58:00.000+01:00

I am making another part using HeeksCNC 0.13.0 and my Sieg KX1.
I made several mistakes and the part is scrap, but I didn't break any tools.
Mistake 1: The clamps were not far enough from the toolpath. I loosened one clamp and moved it and retightened it during cutting. This let the part lift up a little and I cut too deep. I should have pressed STOP, then moved the clamp, then restarted the operation.
Mistake 2: I zeroed the Z of the chamfer tool assuming it comes to a sharp point, but it has a small flat. So the chamfer was cut too big.
Mistake 3: I saw 5 holes and assumed they were all the same size, but some of them were smaller.
I will try again with no mistakes.

Part 0001

2010-04-24T20:04:00.000+01:00

I have made the easiest of the Delrin parts. First I sawed out a piece.
Then I clamped a piece of wood and pocketed an area big enough for the Delrin.
I clamped it down and pocketed a rectangle at z10 with my 6mm slot drill.
Then I changed tool to the 3mm slot drill and pocketed and profiled the holes.
Then I profiled around the outside shape with the 6mm slot drill. The first operation used two depths of cut and left 0.1mm around the outside, climb milling. The second op used one depth of cut and took off the 0.1mm.
I used two tags.
I was pleased with the accuracy. I sawed out the part and sanded off the tags.
All done with HeeksCNC software ( www.heeks.net ). Although I did find some problems and improvements which I had to make to the software before I could get the toolpath.

opencamlib problems

2010-03-29T23:26:00.000+01:00

I found a problem with opencamlib on this cone example this morning and I added an "issue" on opencamlib, hoping to fix it myself tonight, however Anders has already fixed it now.
This was what it looked like before:

This is what it looked like after:

More Zigzag

2010-03-25T10:02:00.001Z

Added material allowance and made start_depth, final_depth and step_down work.

PathDropCutterFinish

2010-03-22T13:13:00.000Z

I changed the ZigZag operation in HeeksCNC to use the new PathDropCutterFinish class that I wrote in opencamlib. This takes samples every 0.1mm along the path and the refines the results so that the final number of moves is reduced within a deviation of 0.1mm. This means that the number of lines of NC code are less, making backplotting faster. In the example pictured, post-processing took about 1 second and then backplotting took about 3 seconds.

BallCutter

2010-03-22T10:11:00.000Z

I tested Anders's new BallCutter class from opencamlib. I did a simple sphere. The picture on the right is where I have moved the sphere down by the tool radius, to show that the toolpath is a sphere.

ZigZag with opencamlib

2010-03-19T04:51:00.001Z

I made the ZigZag operation in HeeksCNC work a bit better with the opencamlib option. This machining library has lots of potential.

Grain the other way

2010-03-18T17:09:00.001Z

This time I rotated the wood 90 degrees and did the same test again (roughing and finishing for both "conventional" and "climb" ).
This time: CV ( conventional ): x width = 19.93mm y width = 19.99mm
CB ( climb ): x width = 20.00mm y width = 20.00mm

So, the grain direction makes a difference. I feel ready for machining the Delrin that I am waiting for.

I have attached some videos to show the difference bewteen roughing and finishing. I guess the noise is indicative of inaccuracy.

Roughing and Finishing

2010-03-18T16:53:00.000Z

No picture, because it would look just like the last one.
This time I did the same test, but duplicated the operations.
I set the original operations to have "extra offset" = 0.2.
I measured the parts at 5mm down from the top.
CV ( conventional ):
x width = 19.99mm
y width = 19.94mm
CB ( climb ):
x width = 20.01mm
y width = 19.98mm

Conclusion: Doing roughing pass, then finishing makes for much better accuracy.
Also: My machine seems to cut smaller in Y, than in X. I wonder if the direction of the grain has any effect? ( I can think of a way to test this ).

Bigger tags

2010-03-18T16:29:00.001Z

I did the same test of "conventional" vs "climb", but with bigger tags. These were programmed as "tag width" = 10mm, so the tags should have been 5mm deep. I measure one, it was 4.97mm deep.
The following measured at about 5mm below the top:
CV
x width = 19.82mm
y width = 19.83mm
CB
x width = 20.09mm
y width = 19.97mm

conventional vs climb

2010-03-18T16:02:00.000Z

I made two profile operations with tags. I notice these tags don't hold the part in very firmly, partly because I made the program assuming the wood is 20mm thick, but it is 19.6mm thick. The tags were set to be only 2.5mm thick, but they turned out to be 2.1mm thick. I could feel a significant amount of wobble in the parts before I broke them out of the block.
I have written CV and CB on them to remind me which was done with conventional milling and which was done with climb milling; for CV the tool went anticlockwise around the square, for CB the tool went clockwise. I used horizontal feedrate of 400 and vertical feedrate of 200.
Measurement taken at a depth of about 5mm below the top.
CV measured:
x width = 19.77mm
y width = 19.82mm
CB measured:
x width = 20.11mm
y width = 20.01mm

This demonstrates how the tool get pulled towards the part with "conventional" but gets pushed away from the part with "climb".

opencamlib

2010-03-18T14:39:00.001Z

I have been trying opencamlib ( http://code.google.com/p/opencamlib/ ). It seems to work OK with a couple of tests. It took 15 seconds to make the NC file for the 10,000 points in the picture. The model made 4084 triangles. It took 25 seconds more to backplot the NC file to see the toolpath in HeeksCNC. I need to change my script to have rapid moves to the clearance plane, before this is useful.

Tags for profile operation

2010-03-16T15:10:00.000Z

I have added the option to program tags in HeeksCNC for the profile operation, by ramping up and down over the tag while cutting the profile.
You can specify the width, angle and number of tags.
They are simply spaced evenly around the length of the profile.
I tested the toolpath by cutting a 20mmx20mm square in some wood.
I was able to cut through the tags with my penknife.
The first video shows a mistake. I had set z = 0 to be at the bottom of the block, instead of at the top of the block as programmed.

More clamping room

2010-03-08T16:46:00.000Z

I need to implement tags on the last cut, so that the part can be held in place.
This part separated when I wasn't expecting it.
It didn't break the tool, luckily.
I have enough done to experiment with drilling the holes on the side.
I have now got a 6mm slot drill, which will quarter the cutting time.

Delrin parts

2010-03-08T14:05:00.000Z

I have been given some step files from someone who wants some parts making from Delrin.
He wants 8 of this part. The first thing is to cut the circle out of the middle.
I haven't got the Delrin, yet, so I am having a go with some wood that I have found in the workshop.

Next to clear the lower level with a pocket operation.
I made the shapes to cut by doing Edge to Sketch, on some circular edges, then making circles with "centre" and "end" ticked in "digitizing". Then I made the circles to sketches, then to faces. Then I subtracted one face from another and made another face from a sketch across the middle, and subtractacted that. Finally I did Face to Sketch to get me the sketches I wanted.
I am doing it all with my 3mm slot drill, so I don't have to set the z height of the tool again. This does mean a lot of tool path, though.

Flyout toolbars improvement

2009-12-01T11:48:00.000Z

Flyout toolbars working OK with Windows, but not quite right with Ubuntu.

OpenGL tree view

2009-11-29T21:42:00.000Z

I made a tree view drawn with OpenGL for HeeksCAD.
This makes it quicker and it doesn't collapse each time something changes.

open source tractor

2009-11-19T15:47:00.000Z

Marcin asks "I was considering Blender. Can HeeksCAD do better?"

I haven't tried Blender for a while.
I like to think that HeeksCAD is easier to use, but that might just be because I wrote it.
Here is a video of me playing with HeeksCAD a few minutes ago.
HeeksCAD has plenty of bugs, but it is OK for making some solid models.
It doesn't do anything nice like fitting solids together.
Save the file every time you do something, preferably with a different file name each time, in case HeeksCAD crashes.

Splines for pocketing

2009-11-14T13:03:00.000Z

Sketches with splines work for pocketing operation too, now.

Spline Machining

2009-11-14T12:39:00.001Z

You can now profile sketches with splines in HeeksCAD ( mostly from SVG file ), without needing to split them into little lines. They are converted into arcs for the python script, but they remain as splines in HeeksCAD. This is in the source code now; http://code.google.com/p/heekscad/source/browse/trunk/src/HSpline.cpp#417 This was inspired by Jeff Epler's biarc code, available here http://bitbucket.org/jst/inkscape-gcode/

BRepAlgo_Fuse

2009-10-21T01:14:00.000+01:00

I added an option "Use old solid fuse" and made it the default. When using the old method, it fixes the problem with unwanted edges.

I found this here http://www.opencascade.org/org/forum/thread_13599/
see 'Use Old Boolean Operations “BRepAlgo_Fuse” can avoid coplanar faces.'

However, apparently the new method is better in other ways, so I have made an option.

OCC offset

2009-09-30T00:11:00.000+01:00

After "geo" from #cam mentioned using Open CASCADE's Test Harness and gave me an example, I produced these offsets, which look promising for pocketing with a permissive license. It seemed to produce the offsets very fast.

flyout toolbars again

2009-09-23T15:37:00.000+01:00

I changed the flyout toolbars to use a popup window with a toolbar in it, instead of the popup menu I was using before. The tooltips don't seem to be working on the Windows version, though.

Graduated Background

2009-09-23T10:22:00.000+01:00

I added a graduated background.
Feel free to suggest some better default colors.
The default is for the color to change from top to bottom, but I have added modes for single color, left to right shaded and four corner color setting.

Flyout toolbars

2009-09-17T17:03:00.001+01:00

I've added fly-outs menu to toolbars in HeeksCAD. Currently you have to press the little arrow button to get the popup menu. Then you have to click again on the menu item. I want it to work with a click and drag, rather than two clicks. Also, I want to get rid of the little arrow button and have click and drag work on the main toolbar button. Also, I want the button on the toolbar to change to the last used tool from the drop-down. I can't work out how to change the tool bitmap, though.

Statistics

2009-08-13T17:48:00.000+01:00

As an owner of a Google Code project, I can set up Google Analytics and see who is looking at the web site. I have done this for HeeksCAD.
You can look at graphs and pie-charts. The coolest thing is the map with the visits shown on it.

Necklace Disc

2009-07-16T19:41:00.000+01:00

I spent the whole day making a necklace thing, made from stainless steel. My girlfriend has a necklace which is made from a piece of shell. It is a circle with a circular hole to put the string through. I measured it and drew it up in HeeksCNC. I added a couple of extra holes to lighten it a bit. I drew some text in Inkscape, wrapped around a curve. I got a bit of 3mm stainless steel from my Dad.
I made two NC files, one for the text and one for the circles.
I set the feedrates to 50.
I broke the tip of my first engraving tool.
I used another stronger engraving tool.
This did the text OK ( at 0.1mm deep ).
I did the text again, another 0.1mm deeper.
I changed the tool to the 3mm slot drill.
Again feedrates at 50. Depth of cut about 0.52mm ( 6 cuts down to 3.1mm deep )
On feeding down, it broke the tool.
I reprogrammed it with feedrates at 10 and bought a new cutter from my dad.
This worked better, but it was too slow to stand and watch. I changed the horizontal feedrate to 25, leaving the vertical feedrate at 10. Later I upped the horizontal feedrate to 40 and it was still OK. Even so, with 6 depths of cut for each profile, it took at least an hour to cut, with me standing there pouring coolant from a jug.

It hadn't cut all the way through, instead it had pushed the steel down into the wood in a bulge. I had to cut through this with a knife.
I filed the sharp edges and sanded it with "Wet and Dry".
The default vertical feedrate should be lower than the horizontal feedrate.
The profile operation, in HeeksCNC, is not remembering the previously entered feedrates.

hpgl in HeeksCNC

2009-07-01T00:31:00.000+01:00

I have started making post-processors for hpgl plotters, for HeeksCNC, after a request from someone called Gary, who has some engraving machines.
In the picture is the toolpath from the sample file that Gary gave me.
I made it so that the machine is now chosen from a drop-down in the program properties.

Code::Blocks

2009-06-23T18:42:00.000+01:00

I made a Code::Blocks project file for HeeksCAD.
I used this on my Dell Inspiron 530 running Ubuntu 9.04.
It works for me. I can edit a file, press "Build" and it only builds the file it needs to.
I can do "Find Declaration of" or "Find Implementation of".
I don't seem to be able to add breakpoints while it's running. I seem to have to add them before I start running.

Drilling

2009-06-15T09:46:00.000+01:00

David Nicholls has added drilling to HeeksCNC.