Newbie- 4th / multiaxis output

[pinguS]

Hi all

Just a quick one, I have been trying the milling tutorials to learn this software. Basically the 2.5D which you can download. All was going well, but then I decided to try outputting Gcode from an exercise, lets say exercise 14.

This in the download has the complete built part, I used the fanuc4ax mac file, which calls the fanuc.gpp

So far so good, but then when reading the Gcode it was only using XYZ, no rotational movements etc. I looked through the gpp file, and notice there is a @fourth_axis in there, but this isn't called unless you do a Transform - 4 axis in solidcam operations.

The solidwork file has been constucted to machine 4 sides of a block, so would have assumed some out of say "G00 C *******" or something along these lines. Not even a machine coordinate is output, i.e. G10 L2 G54 etc...

Can someone shed some light on this, is the post missing something?

[Brakeman Bob]

The short answer is "Yes, the post is missing something". The something in question is some routines to generate code initiated by the changes declared when @tmatrix is output by the CAM.

To generate C or B axis moves you need to set up something that checks if the value you need for your axis of rotation has changed and output the necessary code if it has. However, it isn't that straight forward as the CAM issues @tmatrix twice, before @start_of_job and after @start_of_job and of course if you are using the second one to check if a value has changed the change will not show up using the CHANGE method in GPP because the value changes on the instance before @start_of_job and consequently the change flag sets to FALSE on the call after @start_of_job. Looking back at what I have written it looks more complicated than it is - my advice is if you can structure your NC program to call the pallet rotation before the start of job and therefore sometime the tool change, go for it otherwise there lies ahead some significant post tweaking.

Something to be aware of is when you rotate the part what happens to your MAC and hence your G54 etc. If the part is positioned on the centre of rotation when it is in the machine every is easy but if it is located some distance away from the axis of rotation, say on a tombstone fixture in the case of a HMC, then you have decisions to make about how you handle that.

[pinguS]

Brakeman Bob

Are these things you have already done yourself in the @tmatrix etc?

I have changed on my @tmatrix to just output the new XYZ position after a
i.e. {newX, ' ' ,newY, ' ' ,newZ} just to clarify things when rotated on the X axis

However this still says the machine home_number is 1, so code in places where code is G53 + home_number, is always G54.

Looking at this, i'm assuming the gpp uses G54,G54,G55 etc only for different MAC positions, not positions to each MAC, so if I am rotating around X axis, should I just stick to using aroundX code and update my G54 everytime?

(by the way this is on a VMC with 4th axis in x, (actually its a 5 axis unit, but just trying to get use to 4th axis movement))

hopefully your not confused by what I have just written

[Brakeman Bob]

These are things that I have dabbled with in our posts here, yes, but the bulk of the work was done by SolidCAM UK when we bought the package and susequently added machines.

The machine_home number is driven by the MAC number so when you are setting a CAM job up and you create the first MAC this is MAC 1 - POS 1. Subsequent MAC positions will be on MAC 1 (i.e. MAC 1 - POS 2, MAC 1 - POS 3) unless you tell SolidCAM that you want MAC 2 (or 3 etc.). Of course, you can re-write your post to output G54 for MAC 1 - POS 1 and G55 for MAC 1 - POS 2 if you want; it all depends on the way you want to work. There are lots of ways to program a CNC machine - noe of them is the "right" way, just some approaches are more suitable to some situations. If this sounds like a fudge I'm sorry, I didn't mean it to - what I am trying to say is that is up to you how the code looks because only you know how the machine is going to be run, you know the unwritten rules of of your machine shop (like "G54 = B0, G55 = B90, G56 = B270" to quote one of ours), only you know the different methodologies you deploy.
One of the main reasons I chose SolidCAM is this freedom to configure the post processor to give exactly what we need in terms of code and the way it is called; most CAM systems don't give you that choice or if they do it costs a lot of money.

Back to you question about G54 and the X axis - the short answer is I don't know. You could update G54 for each MAC 1 - POS n or you could (if your control has it) use a G53 local offset. Bear in mind that at sometime you might want to tweak offsets so how do you find them in the middle of a program? Alternatively you could calculate the trig for the cutter position relating to MAC 1 POS 1 and control the tool like that having only a C axis move in the code (by the way, isn't rotation around the X axis defined as an A axis move? the C axis is rotation around the Z). A lot will be hinge on where the part is in relation to the centre of rotation as this is a variable not easily depicted in the CAM. What sort of set up is in your machine? You say it is a five axis, so is it an A & C like our Hermle C20U or is it a "bolt on" like a driven dividing head for A axis mounted on a trunnion for B axis?

[pinguS]

Ours is a trunniun based unit (Nikken) so it uses A and B.

I have been looking for hours and I can't locate the parameter that sapecifies the positions. i.e. Mac 1 - Pos 1 << (parameter for Pos)

I know the Mac parameter is home_number, but where the hell has the Pos one gone? Knowing this makes position setting a hell of a lot easier for the work I would be doing, as I have not advanced to full 5 axis yet.

Also I know this isn't the correct forum, but do you know if Fanuc 18i handles simultaniuos 5 axis or only a max of 4. Currently I can only use 4 simultaniuosly although all 5 can be moved (XYZAB)

Harm

[Brakeman Bob]

Originally Posted by pinguS I have been looking for hours and I can't locate the parameter that sapecifies the positions. i.e. Mac 1 - Pos 1 << (parameter for Pos)

This is the first line of @tmatrix from a "trace" program

(1)@tmatrix ==> mac_number:3 position:1 home_user_name:'G56 B270'

"Mac_number" is the MAC number and "position" is the position

Originally Posted by pinguS Also I know this isn't the correct forum, but do you know if Fanuc 18i handles simultaniuos 5 axis or only a max of 4. Currently I can only use 4 simultaniuosly although all 5 can be moved (XYZAB)

Fanuc 18 can handle 5 axes if you have paid for them and obviously you have as (a) they are visible in the control and (b) you can move them. However 5 axis simultaneous is a different kettle of fish when it comes to programming and Fanuc 18 ain't exactly user friendly as the post needs to calculate all the angular movements in relation to the pivot point, so to create the program you will need the exact distance from the centes of rotation for both A & B to the MAC and the exact tool length & geometry as the tool contact point with the part changes as the angular axes change. Given that, if you want to change a tool offset for a 5 axis job is it can only be done in the CAM and must be reposted. Also, it is a really good idea to position the part so that the MAC (preferably MAC 1 - POS 1) at least lies on one of the axes of rotation at a known distance from the pivot point (or centre of rotation).

Also be aware that 4 & 5 axis moves in Fanuc usually requires the feed rate to be programmed in "inverse time" (the G code of which I don't remember but is in the Fanuc manual) and is called on every line thus

G[inverse time]
G1 X? Y? Z? A? B? Ft

where "t" is the time that the move takes (and the axes all move proportionally to each other).

Creating a five axis post in Fanuc is not for the faint hearted and requires a strong understanding spatial geometry and trigonometry. Good luck.

[pinguS]

Ok wow,

Anyway, i do have the inverse time stuff somewhere, also when i say 5 axis move, if I even program a simple 5 axis movement in 1 line, i get the error too many axis commanded. with 4 it is fine.

I have the fanuc parameter manual to hand as I have changed a fair bit in the past, but never got round to 5 axis stuff, so was just wondering.

[pinguS]

Another quick one, i'm sure your mind has already conquered this, but in 2008, how do you if you can part machine lets say a blank material on a turning process.

Then load that part onto lets say milling with the turning areas complete, like an updated material. (p.s. not turn-mill, but from a lathe setup to a VMC)

I can't seem to save the updated machined part after turning to load into a new milling file??? What a Friday night...

[Brakeman Bob]

Originally Posted by pinguS Another quick one, i'm sure your mind has already conquered this, but in 2008, how do you if you can part machine lets say a blank material on a turning process. Then load that part onto lets say milling with the turning areas complete, like an updated material. (p.s. not turn-mill, but from a lathe setup to a VMC) I can't seem to save the updated machined part after turning to load into a new milling file??? What a Friday night...

Ha, now you are coming up to one of my more frequent rants regarding SolidCAM. The short answer is to save the part machined solid out of the turning SoildVerify as a STL file then reposition its origin / orientation so that you can pick it up in SolidVerify during the milling. I do this all the time as I program OP1 and OP1 for our calipers in two separate SolidCAM parts. To manipulate the STL file generated by the first to be in the right place for the second I use a program called "CtrlView" which was about $45 and does everything I want easily and without fuss. My rant? The fact that I cannot pull the STL file into SolidWorks to manipulate because invariably the STL has too many triangles for SolidWorks to cope with; if you are machining nice curvy surfaces it is not unknow for my parts to have 15 million triangles and up (I think my record is about 38M but that was a killer part). SolidCAM buy SolidVerify from a company called MachineWorks (as indeed do a lot of CAM software companies) so perhaps it is to MachineWorks and to SolidWorks I should be complaining.

[pinguS]

Thanks for the graphics update, I would have expected something simpler, but hey...

Ok, so i've started to mess around with the trunnion set up, no machine graphics as of yet, but now I'm sort of getting use to the tmatrix thing, still confused on the dev_angle_x (y) (z) < what the hell are these, gpp manual is not the easiest to read.

Secondly I've started change the pre processor .mac file, but am confused as to the _5th_axis_around, I know the default is ZYX, but because I have a trunion table fitted on a VMC, so I have set this to YX (I believe writing XY won't work). I chose this assuming that my rotationals are A for rotary and B for tilt of 0-90 deg (although I haven't set the 0-90 in any parameter yet).

However whenever I set an axis in solidcam, lets say on a face at a rotation Y90 Deg, the Z deg also rotates 180 deg and I can't stop this from happening, i.e. I can't flip around the Z. Using setting ZYX this is not a problem. I'm thinking that the YX setting is for mill turn type machines.

God this is started to get complicated.

[Brakeman Bob]

You're right about the GPP manual - it is really more a glossary than a manual. I find when there something I can't quite understand that it is often quicker to post out with "Trace" active and see what is changing after editing the CAM part.

Regarding the machine initialisation settings in the MAC. Be aware that for my 5 axis trunnion machine the following settings apply

_4th_axes_around =
first_rotation_angle = Z
_5th_axes_around = Z
_5x_rotary_axes = ZXY
direction_4x = CW
tilt_axis_dir = CCW

[pinguS]

Ok cheers,

However for curiosity:
My trunnion (sounds rude) at home faces upwards towards the Z axis/spindle. So A is 0(this is rotary). B is 0 (facing upwards), when B goes to 90deg it tilts anti clockwise facing left (like a clock hand dropping from 12 to 9, if this makes sense).

So after a 90 deg move the rotary axis A has moved from being around Z to being around X.

So the big question is, is this trunnion a ZY or XY or does it make it a ZYX.

If ZYX, then when does just ZY or XY, or any 2 axis types apply, I'm sure this is something you have already questioned?

Also if you know, how come your setting for first_rotation_angle and _5th_axes_around are both Z, should these not have been different, ok maybe not in your setup, but when reading the confusing gpp manual, I just assumed they must be different to relate to the 2 different axes's....