Author Topic: Going over to the dark (CNC) side!  (Read 54845 times)

Offline Hugh Currin

  • Full Member
  • ****
  • Posts: 720
  • Box Elder, SD, USA
    • www.currin.us
Re: Going over to the dark (CNC) side!
« Reply #270 on: September 05, 2020, 04:08:48 AM »
kvom:

Excellent. Someone else to ask about Tormach Mesa cards, pin outs, etc.

Thanks.
Hugh

Offline gerritv

  • Full Member
  • ****
  • Posts: 734
  • St Catharines, ON
Re: Going over to the dark (CNC) side!
« Reply #271 on: September 05, 2020, 09:16:22 AM »
Gerrit:

Can't go too far wrong at those prices. I thought it was unobtainable or several hundred dollars. So you're suggesting "PCNC 1100 PathPilot Upgrade Kit - Software & Manual PN: 38706" rather than "PathPilot Software Bootable USB Drive - Recovery Media PN: 38249"? If I can get one I'll start bothering you about which Mesa cards and pin out. But for now which to order. Thanks.

The only downside for Tormach I can see is they'll get more support questions. That could be a problem on their end. Otherwise, win/win.

I confess, I just Google for LinuxCNC questions and end up in the forum more times than not. But it's solid code and free. :-) On my last install I somehow ended up with an old unsupported Ubuntu version which I thought was LinuxCNC's most current release. Works fine until you want to install, say, an editor and all the Repositories are gone. When I get a chance I think I'll upgrade to Mint. Last time around I moved from the parallel port to a Mesa 5I25 card directly connected to my older than old PMDX breakout board.

I tend to be cautious with large scary cnc machines. I use MDI commands and if complex at all CAMBAM. I very seldom hand code G-code, but knowing a little helps at the machine with MDIs. Also handy when modifying post processors. For the mill CAMBAM is, I believe, a good 2 1/2+ CAM package. (I'd like a true 3D package but haven't found one yet.) The CAM packages are pretty good for milling but for lathe work it's a little different. I think there are some good commercial packages for lathe but I can't afford them (and won't use Windows). So, for the lathe I end up doing more hand coding, very carefully. It's a lot easier than a real programming language. A G-code simulator helps with debugging also.

Thanks for the help.
The choice for me was cost, I don't like buying in US and shipping to Canada is extortionate so choose the USB only option. I have a shipping address in NF, NY. (Not much use until next year due to border closure :-() Since my copy is still on 'the other side of the wall', I found a download of the 2.0 version to get on with things.

You have the 5i25 which is directly supported by PathPilot. I went for 7i92 because my Atom PC doesn't have a viable pci slot. The pinout is dictated by which Tormach machine's pinout best matches the PMDX bob. I used jumpers to arrive at the correct match so I avoided editing the HAL files. They get overwritten upon updating PathPilot.

I learned in the early 80's to be OS agnostic, I choose based on what I want/need to do. And for that Windows is far superior to FOSS IMO. I tried Cambam years ago but gave up due to the total absence of the developer for several years. Then came Fusion360 :-) With the Linux subsystem in Windows 10 I can scratch that itch on the rare occassions that I need curl. For Fusion there is also the Mac option although I refuse to spend anything on them :-)

I'll be happy to help once you get to the stage of connecting to the PMDX. I will send you my cable map in a PM, the PMDX-131 should be close to the PMDX-132 that I have.

I am a few weeks away I think from cutting my first chips on this build.

Gerrit
Don't confuse activity with progress

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #272 on: September 20, 2020, 05:01:29 PM »
With the possible loss of some of the F360 functions I thought I should get a few bits that I already had drawn out run through their CAM and knock them out.



First up were a couple of simple 2D contouring jobs being the timing bracket and a knob to lock it's position for teh Thompson engine, couple of holes also done on the CNC for the bracket.



Then the rocker arm for the same engine from steel roughed out with 3D adaptive and then shaped with "steep & Shallow"



Finally the conrod, a rectangular blank was milled down from some round 2014 and the two holes reamed on the manual mill then these holes were used to hold the blank while the 3D adaptive and Steep & shallow did their thing.




Offline gerritv

  • Full Member
  • ****
  • Posts: 734
  • St Catharines, ON
Re: Going over to the dark (CNC) side!
« Reply #273 on: September 20, 2020, 05:51:33 PM »
Very good result. Can't wait to get my machine operational.

Gerrit
Don't confuse activity with progress

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #274 on: November 02, 2020, 07:02:47 PM »
With another stint of pattern making that I can't disclose at the moment out of the way it was time to get back to making metal swarf in the form of the external shaping of a crankcase for a small version of the 36cc Wall 2-stroke.

<a href="https://www.youtube.com/watch?v=D76Bwl9F2gc" target="_blank">http://www.youtube.com/watch?v=D76Bwl9F2gc</a>

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #275 on: November 07, 2020, 04:59:00 PM »
I started this combined inlet and exhaust manifold for the Wall engine yesterday and completed the finish cut on the second side this morning.

First side after adaptive clearing which was done with a 5mm 2-flute cutter for Aluminium from Arc's premium range. Run at 5000rpm, 300mm/min feed, 5mm high x 1mm deep cuts to remove most of the waste then it stepped up 1mm at a time to leave a part looking like this.



Then a "steep and shallow" finish pass with a 4mm dia 2-flute ball nose cutter for aluminium from APT as they do them with a 4mm shank which I needed to reach down the side of the rectangular flange. This was also run at 5000rpm and 300mm/min feed the scallop spacing was set at 0.25mm which takes a while but gives a nice finish.



Then it was basically do it all again for the other side but as the end flanges are different shapes a second setup was used in fusion with the bottom of the work now the top



As it will fit onto the side of the engine. Holes were drilled and tapped while it was still a rectangular block on the manual mill and I was happy that the drilled passages did not appear as the external shape was cut.


Offline Chipmaster

  • Full Member
  • ****
  • Posts: 988
Re: Going over to the dark (CNC) side!
« Reply #276 on: November 07, 2020, 07:34:06 PM »
That's marvellous Jason.

Andy

Offline Hugh Currin

  • Full Member
  • ****
  • Posts: 720
  • Box Elder, SD, USA
    • www.currin.us
Re: Going over to the dark (CNC) side!
« Reply #277 on: November 08, 2020, 03:09:27 AM »
Jason:

Marvelous work and part. I need to learn the software to go beyond 2 1/2 D CAM. Such parts push me in that direction. Very nice.

How did you align the two set-ups so well?

The first picture, first roughing pass is cool by itself. It would make an interesting engine to stop there. Kinda an art deco motif.

Thanks.
Hugh

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #278 on: November 08, 2020, 07:58:26 AM »
It's certainly the type of part where the CNC comes into its own and would mean that all those old aero engine designs that ar eout there with no current source of castings could be made again without needing to spend hours carving manually which I'm sure puts a lot of people off and you have the added bonus of nice material to machine and no chance of finding a defect hiding inside. Makes you wonder if there would be a market for CNC machined "castings" that still left the final machining to the builder?

As for positioning the part. First side was easy as I had machined the block and done the drilling on the manual mill so just set it up on parallels in the vice and located ctr which is what I mostly use a datum and set tool from top of block. For the second side before removing the half machined part I clamped a couple of 1-2-3 blocks in place against the rectangular flange. This then gave me an stop in the X-axis and a vertical face, vice jaw set Y-axis, add a pair of parallels under the two curves and that fixed the parts position.

Offline nj111

  • Full Member
  • ****
  • Posts: 144
Re: Going over to the dark (CNC) side!
« Reply #279 on: November 08, 2020, 11:44:12 AM »
very nice. Could I ask, can those toolpaths be programmed in the free version of Fusion 360 , or is a higher level required?
Nick

Offline Alyn Foundry

  • Full Member
  • ****
  • Posts: 1653
  • North Wales, Great Britain.
Re: Going over to the dark (CNC) side!
« Reply #280 on: November 08, 2020, 12:04:29 PM »
That's marvellous Jason.

Andy

I concur.

 :ThumbsUp:

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #281 on: November 08, 2020, 01:25:27 PM »
I'm not totally sure about the revised "free" version. You certainly won't get it for free as they have moved the "steep and shallow" to what they call an extension which could be purchased for 1 day or 1 months use but I don't know if you can buy it in the free version or only the next level up. The free one I believe will still do the adaptive clearing and there are other finishing options that would come close.

Funny enough The subject came up on ME when someone asked about the new Alibre "Workshop" which is a 1 off payment for Atom3D and MeshCAM though MeshCAM can be bought separately. I had a quick go at the trial version and although it is more basic as you would expect for  alot less outlay it looks like it would give a reasonable finish.

This is the Alibre simulation


And this the MeshCAM simulation, you can see more of a step on the vertical edges in the X direction as it is stepping over in Y rather than stepping along the actual surface.


I've since played about with MeshCAM a bit more and can get a slightly better finish, both examples use a similar stepover. It's something I will need to decide on soon as my access to these features on F360 will soon expire so it's a question of first seeing what I can actually still do in F360 with the new "free" version, paying the yearly fee for a program that I am used to and that has a lot of features or go for something like the one off MeshCAM that is less than a years licence of F360. If I get my finger out and finish off another build article for ME mag then that will pay for a few more years of F360 and Alibre which I use for drawing.
« Last Edit: November 08, 2020, 01:30:18 PM by Jasonb »

Offline Muzzer

  • Full Member
  • ****
  • Posts: 68
Re: Going over to the dark (CNC) side!
« Reply #282 on: November 08, 2020, 03:55:53 PM »
Steep and shallow doesn't allow any particularly unique surfaces to be machined. There are quite a few toolpaths in the free version that can achieve what's being done here (see screenshot) but you'd perhaps need to combine 2 of them.

Most of the other toolpaths tend to be focused on either mostly horizontal or mostly vertical faces. Whilst many of them are capable of machining curved faces, a vertical stepdown or a horizontal stepover isn't best for faces that trasition eg from horizontal to vertical (think a sphere or indeed a horizontal pipe). However, you can tell it to stop when the face reaches a certain inclination. Then you can do the rest with a different, more suitable toolpath. The benefit of steep and shallow is that it achieves a tangential stepover along the surface, so can cope with anything from horizontal to vertical faces. Autodesk consider that enough to command a massive premium.

Looking at Meshcam, I'm guessing the toolpath shown isn't working like SnS - it appears to be running parallel paths. That's one of the simplest of toolpaths and it's one of the many 3D paths in Fusion - if you are doing 3D surfacing, there's not much actually missing in the free version. The main annoyance is the removal of rapids and tool changing (and 4th axis). Having said that, there are already post processor add-ins appearing that get around the rapid and tool change issue.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #283 on: November 08, 2020, 04:25:18 PM »
Although it may not allow unique surfaces to be machined it is the best for this type of work.

It saves having to do parallel in two directions and on a part like that manifold where the vertical edges are at different heights as ringed you really need to run it the full height, its just a simple case of selecting that option and your scallop spacing and it will do the rest so only two items to do the code for - Adaptive and S&S. Before I discovered S&S I was not getting anywhere near as good a surface. But I guess that's why they want to charge a premium for it.

The other MeshCAM option seems to combine parallel in two different directions which is better but won'tt run around and up/down a curve all at the same time though the simulator is not as good as F360 so you can't really see where the tool is moving as it just shows the toolpath and finished surface


Offline Jasonb

  • Full Member
  • *****
  • Posts: 9466
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #284 on: November 12, 2020, 02:39:47 PM »
I had an hour to spare so decided to carve out another casting, this time one of the end plates for the Wall engine, turning of the spigot that locates in teh crankcase and boring for the bearing had already been done in the lathe so just the external shape to be done.

After adaptive clearing and pocketing with a 4mm 3-flute Carbide cutter for aluminium at 5000rpm, 300mm/min feed, 4mm high cut x 1mm stepover on teh adaptive and 1mm x 1mm on the pocket ramping down into the recesses.



Then steep and Shallow while I still can with the boundary set within the inner diameter of the flange, 4mm ball nose 2-flute carbide at 5000rpm, 300mm/min feed 0.3mm stepover.



After that photo I also used the CNC to spot and drill the four 3mm holes. The flange had been left with 0.5mm remaining which I went back to the lathe to turn off.



J

 

SimplePortal 2.3.5 © 2008-2012, SimplePortal