# Proxxon CNC Mill and nccad9 software



## Lofty76 (Feb 10, 2018)

Hello everybody, Recently, in an attempt to get up to date I purchased the above in order to learn some basic cnc programming.Unfortunately the nccad software is mostly in german and support from Max computers (the vendors) is not overly forthcoming. I want to try and learn to manufacture loco nameplates - the ones with raised letters, for a start project.
Can anyone recommend software that will work with the machine and that I can understand?

Many thanks for your help in advance

Regards

Lofty


----------



## kvom (Feb 10, 2018)

I took a look at the nccad/max website.  As far as I can tell nccad is a cam program that works only with imported STL 3D files.  3D machining is probably not what you want for something like nameplates.

Does your machine have a separate control program like Mach3?


----------



## Lofty76 (Feb 11, 2018)

Many thanks for your reply.

The program seems fine for standard engraving, I have worked out to input the machine limits / parameters, setting tool zero height etc, and then running a simple text program ( using a pencil in the machine collet on card clamped to the table), probably not the best way forward but I am beginning to understand the way things work.

I did find a program called VCarve which shows exactly what I want to do. but I can't control the machine from it, the only way that I could see was to export the vcarve code into the nccad program as the trial version of vcarve doesn't allow export directly to the machine.

Does Mach 3 have a usable trial?


----------



## kvom (Feb 11, 2018)

As long as g-code can be imported to the control that's the way to go.


----------



## Lofty76 (Feb 18, 2018)

Thanks Kvom, Mach 3 works a treat, much obliged.


----------



## Chris Alderson (Sep 23, 2018)

Lofty76

I currently have the same problem you where experiencing, I have just purchased the proxxon ff 500 cnc which comes with nccad9

However the software that is provided with the system is only the basic version with lots of restrictions, I have looked in to upgrading it to the full version which is going to cost another £290 that's without shipping as you can't download it they have to send you a CD probably because they charge you another 280 euros for international shipping.

Any advice on software alternatives or just a direction to head in here would be a life saver because nccad9 basic is just about unusable and has no 3d functions or useful help.

Any assistance will be greatly appreciated 

Chris


----------



## Bazzer (Sep 23, 2018)

Chris Alderson said:


> Lofty76
> 
> I currently have the same problem you where experiencing, I have just purchased the proxxon ff 500 cnc which comes with nccad9
> 
> ...


Chris

I have a Wabeco CC F1210 mill that runs with NCCAD 7.5, I get a lot of work out of the machine and NCCAD.

I do not however try to do any 2D or 3D CAD within NCCAD, just regard NCCAD as a machine control like Mach3 or Eding and import G code generated by another CAD/CAM program.

You will not be able to get anything like Mach3 to drive the Max computer controls, they have that side of things locked down very tightly.

The accepted G codes for NCCAD are fairly limited, however you will be able to make the machine do just about anything that you want, you will have to get a post processor sorted out if you do use another CAD/CAM to generate designs and G code.

I did have a little communication with Max Computer about 3D capabilities and in his very broken english he said anything complicated to generate outside of NCCAD and import the G code.

Anyhelp or sample code required then just drop me a line, I am 99% certain that the code is identical for the wabeco and proxxon versions.

Regards

Barrie


----------



## Chris Alderson (Sep 23, 2018)

Hi Barrie

Thank you for replying

The version of nccad9 I have received with the proxxon FF500/bl cnc is nccad9 basic which has very limited usability.

You cant import stl files, you can only open 1 file at a time, and you cant generate anything over 5000 sentences as they put it.

Currently I have tried simple engraving and never get past the first letter, I get an error message, and there is nothing to check this error message against, nothing about it in the help directory which is honestly useless as it refers to the full version of nccad9.

I have looked in to upgrading nccad9 to the full version which I really shouldn't have to do as I've paid over £5000 for this machine and software and the cost including shipping would be well over 500 euros because you cant just download it from them they have to ship to to you, which I'm definitely not going to pay on top of what I already have.

I posted on here as it seems Lofty76 got some joy with Mach3 ?

Regards

Chris


----------



## Bazzer (Sep 23, 2018)

Chris Alderson said:


> Hi Barrie
> 
> Thank you for replying
> 
> ...


Hello Chris

5000 lines maybe a limitation, I dont do engraving so I dont know how many letters 5000 lines buy you.

I bought the hand pendant direct from Max computer, they dont charge the 280 euros shipping, I think that is to cover themselves for tricky exports, get a shipping quote from them, it will be 20 euro's or similar.

I would definately be interested to know if some one has the key to get the Max computer control working with Mach 3 but I am not holdig my breath on that one.

The best thing to do is make the mill follow a really simple programme to start with, that proves everythings out.

G91
G00 x100
y30
x-100
y-30

Create the above programme in notepad or similar and save the file with the extension *.KNC,  so change the file you create in Notepad from having *.txt to KNC.  Set your machine zero point so as that there is plenty of movement avaliable in the positive X axis (table quite well over to the right) and with the table fairly close to you to allow movement in the Y axis, leave the Z axis up high. Zero the machine by pressing ctrl X, then ctrl Y and finally ctrl Z. 

Now open the above created file and press the go button and see what happens. If you get this going I can walk you through getting a bit more adventurous !!

I hate to say this but you have to get this working, I will bet you that it is not possible to get the controls working with Mach 3 so you have to keep going. I use the NCCAD controlled Wabeco more or less every day, there is a learning curve but it is all possible. I do mostly 3D machining of stainless steel. Where did you buy the mill from?

Regards

Barrie


----------



## Chris Alderson (Sep 23, 2018)

Hi Barrie

I have done as you advised, the 5000 lines is for any job engraving was just a quick test of the machine to see if it functioned as expected but didn't work, as soon as the first letter is machined the program throws up a z axis invalid move error and ends, I tried this with basic shapes and get exactly the same result, z axis movement error.

There is nothing to refer to for causes of this error at least not that is in English.

The code you game me made the x and y axis move, looked like the table was stencilling out a rectangle, no movement on the Z axis at all.

Regards

Chris


----------



## ThomasSK (Sep 23, 2018)

What is your safe Z set to? lets say you have a mill with 200mm of Z travel, and you send it a g-code like "Z-1000" then your controller may throw a error like that. 

I'd recommend reading one of the basic courses of programming G-code. With the cheat list of M and G codes, its fairly easy to do the basic shapes, and its quote helpful when you are fault finding a program.

As a test, lets try this program:

```
G21
G90
M3 S1000
G00 X0 Y0 Z0
G01 Z-1
G01 X10
G01 Y10
G01 X0
G01 Y0
G00 Z-10
M5
M30
```
This should start in one corner, start the spindle at 1000 rpm, go down 1mm, then go 10mm in X, then 10mm in Y, then  back to make it a square. 
I'm not sure that the proxxon has control of the spindle from the controller, in that case, remove the S1000 from line 3. 

Wikipedia has a good list of what the codes means

BR.
Thomas.


----------



## Bazzer (Sep 23, 2018)

ThomasSK said:


> What is your safe Z set to? lets say you have a mill with 200mm of Z travel, and you send it a g-code like "Z-1000" then your controller may throw a error like that.
> 
> I'd recommend reading one of the basic courses of programming G-code. With the cheat list of M and G codes, its fairly easy to do the basic shapes, and its quote helpful when you are fault finding a program.
> 
> ...



Thomas

This machine has a funny implimemtation of DIN ISO G codes, it will not start or stop the spindle with M3 and M5, G21 will not be recognised, M30 will throw it as well as they use M30 as a pause and then you specify the time delay of the pause.

Spindle start is M10 o6.1 and stop is M10 o6.0 

The characters in front of the 6's above are letter 'O' for output.

Very strange controls but used by two well respected German manufacturers, go figure.

Best Regards

Barrie


----------



## kf2qd (Sep 23, 2018)

Can you tell uswhat G and M codes the machine accepts? And what CAD system you might have experience with?


----------



## Bazzer (Sep 23, 2018)

Chris Alderson said:


> Hi Barrie
> 
> I have done as you advised, the 5000 lines is for any job engraving was just a quick test of the machine to see if it functioned as expected but didn't work, as soon as the first letter is machined the program throws up a z axis invalid move error and ends, I tried this with basic shapes and get exactly the same result, z axis movement error.
> 
> ...



Hello Chris

As Thomas eluded to the Z axis error you are getting is likely to do with the Z zero and travels conflicting.

So set the Z zero with the Z axis about half way up the Z travel movement.

Now run this code

G91
G00 X0 Y0 Z0
Z -10
x100
y30
x-100
y-30
z 10

You will see the same rectangle as before but the Z axis will drop 10mm at the start and raise 10mm at the end.

Also as a seperate programme try this

M10 O6.1
M30 p180
M10 O6.0

This programme starts and stops the spindle with the Wabeco mill, it might be different for Proxxon, let us know what the results are of the spindle test, M10 is relay controls in NCCAD speak. 'O' (letter O) is output 6.1 is relay 'on' and 6.0 is relay 'off'. M30 is pause and the P180 is pause for ten seconds, they split a second down into 18th's so 10x18 equals 180.

With the Wabeco the spindle speed is set manually, I think the Proxxon is the same looking at the photo's.

If the above is all ok then I think we should cut some material, do you have some 3mm plywood? what cutters do you have? Looking at the spec of the machine on the Proxxon website it looks like the spindle RPM is max 2500 rpm, is that your understanding? I see they offer a bracket to get a high RPM spindle mounted, that sounds like a good idea to me.

One step at a time as they say!!

Best Regards

Barrie


----------



## Chris Alderson (Sep 24, 2018)

Hi Barrie

I loaded the program in to nccad it seems the pieces of code for the Z axis movement had spaces in as the system gave an error for each line, I've taken the spaces out and all seems to be ok.

The code ran fine Z dropped, X and Y made a rectangle but when Z was returning to the 0 point it ran very slowly, no doubt this is a setting somewhere ?

kf2qd I currently have no experience with G-code other than the above Barrie has kindly shown me, I'm only just getting in to CNC so baby steps at the moment, I have used google SketchUp quite a bit, years a go I used 3ds max but that was a good while back.

I have been looking in to different CAD programs to use for design then being able to import in to nccad9 but because of the restrictions on nccad9 basic I'm not really able to do this, plus forgive me if I'm wrong but nccad doesn't really seem compatible with other programs ? perhaps this is just the fact I'm using the basic version ?

Thank you for replying to me so promptly everyone, I didn't think I would receive a response so soon never mind all the help I'm receiving plus the G-code lessons im getting from Barrie.

Regards

Chris


----------



## Bazzer (Sep 24, 2018)

Chris Alderson said:


> Hi Barrie
> 
> I loaded the program in to nccad it seems the pieces of code for the Z axis movement had spaces in as the system gave an error for each line, I've taken the spaces out and all seems to be ok.
> 
> ...



Hello Chris

Not sure why it went slowly in the Z rectract, once G00 is invoked (rapid movement) the machine should stay in that speed until G01 is invoked (G01 is move at cutting speed) we did not call up G01, so that is strange. Did you get to try the spindle start and stop programme yet? and did you get a chance to look for materials and cutters?

Let me know if you wish to continue this remote tutorial and we should be able to get 2.5D cutting going quite easily, then maybe flip back to trying the engraving within NCCAD.

NCCAD is not the most friendly programme to start with but you can get things done with it, Wabeco and Proxxon sell a good number of machines with this software.

Out of interest where did you buy the Proxxon machine?

Best Regards

Barrie


----------



## Chris Alderson (Sep 24, 2018)

Hi Barry

I believe it may be a setting somewhere.

Yes the spindle program worked fine no X,Y or Z movement just spindle on and off, so from that I'm getting M10 O6.1 tells the MCS control unit to close relay 6 (Close contact) and M10 O6.0 open relay 6 (Open contact).

I have Aluminium sheet, loads of scrap pieces of Pine, Steel square bar, Brass round bar.

Endmill cutters HSS 6, 7, 8, 10mm 4 flute / Tungsten carbide 6mm 4 flute and proxxon milling cutter set 1, 2, 3mm 2 flute 
I also have a few other cutters Axminister's own make they are more like rasp cutters though.

I bought the machine from Axminster tools and machinery.

By all means Barrie please continue the tutorials as it is really helping with my understanding of the CNC machine and how G-code works in relation to it.

Regards

Chris


----------



## Bazzer (Sep 24, 2018)

Hello Chris

Your understanding of M10 and the relay sense is perfect. I take it that the speed of the spindle is set manually?

If you want to cut a part, I would propose a rectangle with a circle or ellipse cut out of the middle. Given that the machine is new and feed rates are a bit of an unknown I would strongly suggest cutting some plywood or similar material to start with. you have cutters listed that would be just fine for this test. We do need to know the thickness of the work piece material if we are going to cut it free. Alternatively we could mount a lump of pine into the vise if you have one and work away above the vice jaws.

If we do a flat sheet job we will need a sacrificial board underneath the work piece, 10mm ply or MDF is good for this, but you need some kind of clamp system to hold the boards down onto the machine table.

I looked at some videos of the machine that you have on Youtube doing engraving, the machine seemed quite capable.

Let me know on the questions above and I will get something programmed up for you.

Best Regards

Barrie


----------



## Chris Alderson (Sep 24, 2018)

Hi Barrie

Yes the speed of the spindle is set manually on the front of the machine head, it peaks at 4000 rpm.

That would be great Barrie if it is not too much trouble, I can get the material ready, also I have a set of step clamps to hold in place.

Yes I have probably watched the same videos however I now know the 5000 sentence limitation of nccad9 which I managed to fill with one 5 letter word at a 2mm depth which I find ridiculous, I did speak to proxxon via email earlier on today and they tried to advise me they have only provided basic to try and keep the cost of the machine down. They also went on to say that it should satisfy most tasks other than the use of STL files.  Guessing the gent who emailed me has not yet tried to engrave on basic..

While I was making my discovery earlier I received that "invalid movement z axis" message again and from what I can gather it is happing somewhere in these lines of code:

G01 X48.965 Y30.284
G01 X48.130 Y30.360
G00 Z5.000
G00 Z0.500
G01 Z-2.000 F5.000
G01 X48.320 Y30.990 F50.000
G01 X59.790
G01 X59.600 Y30.360
G01 X58.996 Y30.331

Any ideas what could be causing this error Barrie ?

Regards 

Chris


----------



## Bazzer (Sep 24, 2018)

Chris Alderson said:


> Hi Barrie
> 
> Yes the speed of the spindle is set manually on the front of the machine head, it peaks at 4000 rpm.
> 
> ...



Hello Chris

Lets look at what the code is telling the machine to do.

G01 X48.965 Y30.284 This line is a cutting action, assume the tool is cutting and it is going to X 48.965 and Y 30.284
G01 X48.130 Y30.360 Cutting action again with a very small movement relative to the last line
G00 Z5.000 This is a rapid movement pulling up in the Z axis 5mm away from the zero point
G00 Z0.500 This is a rapid movement but looks to be 0.5mm above the work piece.
G01 Z-2.000 F5.000 This a cutting/plunge action into the work piece at a feed of 5.0 (actually 30mm/min)
G01 X48.320 Y30.990 F50.000 Cutting in the X,Y plane with cutter at the depth from the previous line feed of 300mm/min
G01 X59.790 Cutting movement just in the X axis
G01 X59.600 Y30.360 Cutting movement
G01 X58.996 Y30.331 Cutting movement

Another qwerk of the Max computer control is that the feed rate (F after a cutting operation such as G01) unit is 0.1mm per second rather than the more convemntional units of 1mm second. so F5 in your code is 0.5mm per second which works at the more conventionally quoted figure of 30mm/min. Basically multiply Max computer feed by 6 to get a mm/min figure.

I see nothing outlandish in your code but if you had the Z zero set very close to either the top or bottom of Z axis travel, then one of the Z axis movement requests could push the machine out of limits and result in the error message. Try running the code again but set the Z axis zero right in the middle of the travel. Have you got the Z zero set very low on the Z axis, maybe a very short cutter has forced you to do this?

I assume the code was some sort of engraving or text?

Did you speak to Axminster about any of this? I would be interested to know if they have someone down there who understands the qwerks of Max computer controls?

I will figure out the programme tomorrow but feel free to ask any questions that come to mind before then.

Best Regards

Barrie


----------



## Chris Alderson (Sep 24, 2018)

Yes I was able to get my head around most of the code and figure out what instructions where being sent to the mill apart form the max computer feed rate conversion.

This is part of the code generated by the NC-program in nccad9 for a simple engraving of 4 letters using a 0.5mm engraving bit, as far as I can tell the issue is when the first letter is finished and the machine is moving to the next letter, it lifts on the Z axis, drops on the Z axis and before moving stops and gives the above error.

what puzzles me is the fact it starts and finishes the first letter fine then gives the error when moving to the next.

I have not spoke to Axminister regarding this but will be at some point regarding the description on the website for this machine, I have to say I have only ever had good experiences with purchasing form Axminister however.

Barrie do you use a program to generate the code or do you just write it your self from scratch ?

Regards

Chris


----------



## Bazzer (Sep 24, 2018)

Hello Chris 

I rarely write programmes by hand, I generate code in a programme called BobCAD, sometimes I do the 3D designs in BobCAD and sometimes in other programmes such as Alibre Design or MOI.

Mostly I like making RC pylon race aircraft, the wing and tailplanes of the models in the photo's are designed by me and machined by me and the younger guy, he is an excellant machinist. The wing has 2.8 million lines of G code to produce male patterns.

These models fly at around 200mph and have a very powerful 6.5cc engine






I think that Axminster just use the text from Proxxon to describe the products on their website, I think there is quite a learning curve with any CNC system, the problem with Proxxon and Wabeco is that they dont have a big presence in the English speaking World with their CNC offering so it is not easy to find people to ask questions and bounce ideas off of.

I already had a fair understanding of G code and CNC in general, so in about a day I had figured out the qwerks of the Max computer controls.

I guess you either have to ***** like hell to Axminster and I doubt they will do anything or alternatively keep calm and politely point out the failings but get on and learn the system. I think you will get there quite quickly as you are able to figure stuff out.

Would you upload that whole engraving KNC file for me to have a look at?

Best Regards

Barrie


----------



## Chris Alderson (Sep 24, 2018)

Hi Barrie

I will have to take a look at those programs, I have no doubt they will come in handy as I have already looked in to so many from cad to cam to generate g code to import in to nccad, it really has gave me a headache.

Ah I see, my older brother got in to RC when we where quite young he had an over wing trainer with a decent little OC engine that ran on nitro methane if I remember rightly, wasn't the best smelling fuel, he also got in to flying helicopters and was a big fan of RC cars too although he never got a chance to get in to the engineering side of them.

I had somewhat of an interest in them at a younger age but migrated towards computers and learning as much as I could about them, I work as an electrician and am currently now doing an HNC in electrical engineering as well, I'm getting in to CNC as more of a hobby than anything else although I've seen quite a few uses where it will come in handy.

Yes they do Barrie, I noticed that when originally looking in to this machine and viewing the details of it on both websites, I've been dealing very closely with a gent who works in my local store all the way through ordering this machine, he has went way beyond the expected realm of customer service even delivering the machine to my door him self and helping me carry it in to were I set it up.

Axminster have been very forthcoming with information I have requested and had advised me there is somewhat of a delay from me asking a question to them receiving a reply from proxxon as any information asked is really 3rd hand information, its much easier to just email proxxon.

I plan to stick it out as I really do think the machine its self is of excellent quality and will probably just take more of an understanding of the control side of the equation to get everything working as I want, granted its a bit of a strain at the moment as learning this on top of quantitative methods, dimensional analysis and the programming of PLC gives one somewhat of a headache to say the least.

I will have a go at uploading it Barrie but not sure if the will be a limit to the characters I can enter in a post on here, the file is quite large in terms of character count.

Regards

Chris


----------



## Chris Alderson (Sep 24, 2018)

Here is the file Barry, I didn't realise I could just upload the file itself, please find it attached.

Also if you are wondering who Jack is which is what the engraving spells out he is my Yellow thighed caique.

Regards

Chris


----------



## Cogsy (Sep 24, 2018)

Just for some piece of mind Chris - that file you uploaded would count as 1182 'sentences' only, so you're not hitting that limit. That should also give you an idea of how big a job you could get done with the basic version of your software. When I was using a trial version of MACH 3 it was limited to only 500 lines (sentences) but even so I could engrave a fairly detailed scorpion. 5000 might well be enough for you, especially if you chain programs together when you get to a very complex part. For example, the first program could carve out one side of a flywheel, the next engrave the outer rim or something like that.
I'm thinking it's as Barrie suggested, you are operating at one end of your allowable Z travel and the command to lift the cutter out of the first letter is trying to exceed the allowable limit, causing the crash.


----------



## Chris Alderson (Sep 25, 2018)

Hi Cogsy

I see 1182 is a lot less than 5000, however if I add just a few more letters, it flags up with an error saying I'm exceeding the 5000 limit and cuts off which ever letter came last.

I wouldn't have minded had I known the basic version came with the machine and not the full version when I was looking in to purchasing it, however when looking at the information on proxxons website there is no indication of this at all which to me is misleading, you only find out once you have installed the software and try to update, or go to proxxons website, click on the software update link on the page for this machine, it tells you straight away that you only have nccad9 basic and if you want to use the full program you will need to go to the shop.

I see, so where do I check the allowable Z travel limit ?

Regards

Chris


----------



## Cogsy (Sep 26, 2018)

I agree they should make it clear - seems a bit dodgy to me as well. 5000 lines is quite a bit in the CAM software I've used in the past, such as CAMBAM, but yours may be different. I just checked an example I made a while back, a Christmas bell mold I made. The bell itself was 4 different heights, with around 6 pocketing passes to achieve the depths, plus at least 2 passes of text engraving which read (in fancy script) "Merry Christmas 2014 from the FAMILY_NAME family" and in total it was 3096 lines of G-code.

I can't help you with your Z limits as I don't have any experience with your machine/software. What I'm used to  is a button in the controller software that allows you to define a zero, then coded limits for allowable travel which you tune for your machine. It's quite possible that yours is set to only a small allowable positive Z value and the error will be generated when a call to go above that is executed.

Looking at the code you uploaded where you think the error is occurring for you, there is a call to retract the Z to 5mm above zero. If your maximum allowable Z value is anything less that it will create the error you're seeing. Maybe try searching through your settings to find anything about limits. Also, there is a thing called "soft limits" which is where the machine will slow down its movement speeds when approaching the limit of travel, so as not to bang into any stops due to inertia. If you have this setting enabled and your Z limit is close to zero it would explain why the rapid Z retract in Barrie's code was a slow retract. BTW - Barrie is much more familiar with this stuff than me, I was just making a suggestion. Trust his input more than mine!


----------



## xpylonracer (Sep 26, 2018)

There are several incidences of code raising the cutter out of the work to 5.0 and then moving to 0.5 before applying a cutting depth move. I take it Z00 is the workpiece surface.
G00 Z5.000
G00 Z0.500
G01 Z-2.000 F5.000
What's the point of the first 2 lines in the above code ?
If no positioning move or tool speed/direction change why raise the tool ?

Emgee


----------



## Chris Alderson (Sep 26, 2018)

Hi Cogsy

I ma going to persevere and see how it goes, Axminster are chasing up possibly getting the full version of the software shipped over for me but just waiting on them getting back to me.

Either way I appreciate your input, any knowledge is good knowledge.

xpylonracer, I'm not totally sure from what Barrie has shown me so far G00 is rapid movement so the Z axis is being told to move up 5mm above zero point but then to move back down to 0.5mm above zero which seems a waste of time due to there being no x or y positional change, then G01 (move at set feed speed), Z-2.000 (Move Z axis to -2mm below set zero point), F5.000 (move at set feed speed of 5.000).

Please correct me if I have made any mistakes above.

I noticed this on another programm where nccad had entered G00 Z20.000 then G00 Z20.000 straight after repeating the same line of code.

It may sound a bit daft but it wouldn't surprise me if Max computer had set this up in order to use the 5000 limit quicker in the basic version to increase frustration and likelihood you will go and give them another £290 quid plus shipping, I know it sounds a little far fetched but they do seem the type from what I have read on them so far. 

Regards 

Chris


----------



## Bazzer (Sep 27, 2018)

Chris Alderson said:


> Hi Cogsy
> 
> I ma going to persevere and see how it goes, Axminster are chasing up possibly getting the full version of the software shipped over for me but just waiting on them getting back to me.
> 
> ...


Hello Chris

I will try and get a sample code set done for you this evening.

Regarding Max Computer, I dont think they are particulary cunning or sophisticated so I doubt any clever conspiracy theories. They survive by providing software that is taken up by the education sector in Germany in my opinion. They are OK to deal with commercially.

I think the Proxxon published information about NCCAD 9 is vauge at best, Wabeo clearly have a table of limitations of the basic v pro versions of the software.

I think you are left with little choice but to upgrade otherwise you will always be hitting this 5000 line limit, I know it hurts a little to be facing another cost but if the machine had been presented to you costing £280 more you would have probably still bought it, just saying.


Best Regards

Barrie


----------



## Bazzer (Sep 27, 2018)

xpylonracer said:


> There are several incidences of code raising the cutter out of the work to 5.0 and then moving to 0.5 before applying a cutting depth move. I take it Z00 is the workpiece surface.
> G00 Z5.000
> G00 Z0.500
> G01 Z-2.000 F5.000
> ...



Emgee

That sort of thing can happen with CAM and post processors, the CAM see's some area it wants to machine and maybe close or next to and existing cut but it see's that it has to unengage the cut, hence the positive Z axis movement.

I have to say though, I did not see such movements in the 2.8 Million lines of code for the wing !!

Best Regards

Barrie


----------



## Bazzer (Sep 27, 2018)

Chris Alderson said:


> Hi Cogsy
> 
> I ma going to persevere and see how it goes, Axminster are chasing up possibly getting the full version of the software shipped over for me but just waiting on them getting back to me.
> 
> ...


Hello Chris

Cogsy might have a point regarding setup of the Z axis travel, if the Z axis travel number is incorrectly set very low then the machine could just run out of travel.

Are you able to manually drive the Z axis down to the table with a cutter in place (mind the table). 

I have attached a screen shot of the area where the Z axis travel is set, look for menu item Parameters>Machine and this is on the first tab/page.

Best Regards

Barrie


----------



## Bazzer (Sep 27, 2018)

Chris Alderson said:


> Hi Cogsy
> 
> I ma going to persevere and see how it goes, Axminster are chasing up possibly getting the full version of the software shipped over for me but just waiting on them getting back to me.
> 
> ...



Hello Chris

Of course one thing that none of us have mentioned, especially seeing as how you are self commisioning the machine, has some kind of referance run been done to find the machine home positions.

on some hobby machines this just means carefully running the machine up against mechanical stops (Stepfour 540 basic router and EMCO F1 mill springs to mind) but I have a hunch your machine has switches as Max Computer has a 'Go to referance point'  button when you are in the machine control.

On the Wabeco that is the first thing I do when starting the machine up.

Regards

Barrie


----------



## Chris Alderson (Sep 27, 2018)

= Hi Barrie

That would be very much appreciated.

To be honest I don't think proxxon are too bothered, I received a reply today basically saying sorry nothing we can do basically referring me to MAX-Computer again.
If I had been offered the upgrade at point of sale I would of taken it hands down, Unfortunately I was under the impression that the machine would be working to its fullest potential in 3 axis out of the box, on the software it came with.

lesson learned is all I can say.

I've had a look at the values you have shown me in the screen shot Barrie and am a bit confused as they are as follows:

X = 285
Y = 103
Z = 195

In the manual the traverse paths are as follows:

X = 290
Y = 100
Z = 220

However looking at the specs for the machine its self online the traverse paths should be:

X = 220
Y = 100
Z = 290

Which would make sense as the Z axis is massive in comparison to the other 2 on the machine, not sure what to do there ?

Do you think the above could be related to the error ?

Regards 

Chris


----------



## Chris Alderson (Sep 27, 2018)

Yes that was one of the first things to do in commissioning in the manual, go to home position (End switches)


----------



## Bazzer (Sep 27, 2018)

Chris Alderson said:


> = Hi Barrie
> 
> That would be very much appreciated.
> 
> ...



Hello Chris 

I think we might be getting somewhere!!

The machine will  home in the Z axis at the top of the Z column, if the machine is only being allowed to come down 195mm from that position, you may well be trying to work right at the limit of it's imposed shorter travel.

I would set your Z zero half up the Z axis column and run the engraving programme again, my guess is that it will work.

Without seeing the machine up close it is a bit difficult to setup that Z axis travel, however I would proceed as follows.

Do the 'go to home position' run, and zero the Z axis in that position then drive the Z axis down with the cursor keys or the down arrow in the machines software control panel. Very likely it will stop at 195mm, this will show in the readout. Be careful that nothing is in the way or obstructing the machine as it comes down.

If everything happens as described above then start altering that 195mm figure in the setup towards 220mm, you will have to look at the machine etc to be sure that nothing stupid is going to happen like crashing into the table !!

The Wabeco is set in such a way that the spindle with no tooling loaded cannot peck at the machine table if that makes sense.

No chance to do the programming tonight - sorry

Once you have the Z axis undercontrol it would be normal to zero the Z axis on either the top or bottom of the work piece, in Max Computer you ahve 20 diferent work piece zero points, this is handy for running different jobs.

Best regards

Barrie


----------



## Chris Alderson (Sep 27, 2018)

Hi Barrie

I know once I had commissioned the machine I had a little go moving the Axis with the cursor keys inside manual control, I did notice the Z axis stopped well above the table and would not go any further which puzzled me, but I believed at the time a mistake like that would not be made at the factory.

Also the table movement on the X axis is not even, when the table moves to the right I worry about load on it as it stretches right out and partially runs off the dovetail slide ways, but the other way it hits the limit switch. no where near as far over as the opposite direction.

I actually tried jacking the work piece up 30mm and had no problems at all, the same program ran to end with no problems.

The original piece's top face was already lifted 60mm off the table surface.

When ever you get a chance would be great Barrie, I'm currently messing round with a plugin I found for sketchup which generates G-code for the object you make in it, there are a few kinks to iron out though as I'm modifying the script to use KOSY friendly G-code which it currently doesn't  so have just been modifying it post process before importing to nccad, seems to work ok once it has been tweaked though.

I will have to get my head around the 20 different workpiece zero points and their uses.

Regards 

Chris


----------



## Bazzer (Sep 28, 2018)

Chris Alderson said:


> Hi Barrie
> 
> I know once I had commissioned the machine I had a little go moving the Axis with the cursor keys inside manual control, I did notice the Z axis stopped well above the table and would not go any further which puzzled me, but I believed at the time a mistake like that would not be made at the factory.
> 
> ...



Hello Chris

From what you have said I think we can say that all of your problems have been an in correctly set Z axis travel.

If we look at your numbers it tells the story, so you raised your work piece by 30mm then the prgramme ran, so what you effectively done was put the workpiece into the catchment area of the 195mm  travel limit.

I would then further suggest that the travel limit will likely need extending towards 280mm if you are going to be able to work with flat sheet materials sat on top of a spoil board on the machine table.

I will address the issue of the table running off the dovetails this evening.

If you tweek that Z axis travel limit in the software, then I think you are home and dry !

Best Regards

Barrie


----------



## Chris Alderson (Sep 28, 2018)

Hi Barrie

I have checked the set limit values and they are correct, the Z axis is not able to run any further down toward the table than its set limit sounds like it jumps off the screw threads if tried, its not really a problem I can just lift the work piece up in future, just glad I now know what was causing the error in the first place.

Regards

Chris


----------



## tjwal (Sep 29, 2018)

Estlcam.de is a simple cam product that is easy to use and UNDERSTAND.  It opens and displays a dxf file.  You then choose one of the shapes and through a menu and icon system you tell it what you want.  For example for a rectangle you can cut around the outside, inside or clear out the inside.  You choose the tool and federate to use.  It takes this info and generates gcode.  I found it useful to generate gcode for a few different shapes and the exam the gcode and figure out what it meant.  A great way to learn gcode!
It’s free to use but after a number of uses a timer pops up suggesting that you license it.  I think it’s only $50.


----------

