Post for a SCM Record 220 with NUM 1080

[Anonymous]

Hi,

We are looking to fully integrate Fusion360 into our design process and utilize its CAM fuctionality, wanted to see is anyone has a post processor for a SCM Record 220 with a NUM1080 controller?

Thanks!

[bob.schultz]

Hello Cameron,

As you can see in the snippet of output in my previous post, Fusion is not breaking up the circle into XY-moves, but is actually outputting G02 and G03 blocks for the contour motion.  Do you have different output than what I posted here?  I don't see any XY contouring moves in the output I produced from your sample part.  Please furnish me with the code you are getting from Fusion and from Alphacam.

Thanks,

Bob

[Anonymous]

Hey Bob, 

Going to be working to get a part and corresponding G Code for Alphacam and Fusion shortly. Based off what you were saying earlier, does fusion only output radial commands for lead in and lead outs? 

Thanks Again for the Help,

Cameron

[bob.schultz]

Hello Cameron,

Fusion will output circular arcs when appropriate.  In a previous post I showed you the circular arcs I was getting with the profile motion.

(Contour motion)
N50 G02 Y3.162 I1.456 J1.456
N51 Y-0.25 I1.456 J1.456

Running the last part that you sent to me along with the latest post, you should also be getting this output.

[Anonymous]

Hey Bob,

Just ran a part with the a bit that should have been spinning counter clockwise based off my parameters set in fusion. When I ran it however, the bit spun clockwise. Wondering if there is something in the post that is not acting properly. Thoughts?

Thanks Bob!

[bob.schultz]

Hello Cameron,

Yes, it seems the post is hard coded to output an M3 with the spindle speed.  Here is an updated post that fixes this problem.

Bob

[George-Roberts]

Just as an addition to this, tick the smoothing option in the operation (passes tab) to generate more arcs, that should reduce the code

[Anonymous]

Hey George,

Always run it with smoothing on because it was causing data starving at the machine every time when I was not. However, I have read some things about what the ratio between smoothing and tolerance should be. Right now I am running smoothing at the same value as my tolerance (0.005), most of the time there is no problem, but any thoughts on what a better ratio might be?

[Anonymous]

Hey Bob,

I believe I had mentioned this before, but we have had some problem with data starving on our machine while running fusion 360. We looked at the G code from Fusion and from our old program and we noticed that there is an extra digit being generated in fusion. Instead of for example 0.001 it is generating as 0.0015. The machine is only accurate to within 0.005 so this extra digit is insignificant to us. My initial thought is that this is adding extra precision that is causing the machine to lag. I then looked at the most recent post we received and found under capabilities and tolerances that the tolerance is set to spatial (0.002,MM) if this is setting the tolerance at 0.002mm that is well beyond the precision we can achieve. Would it be possible for you to update the tolerance section to reflect a machining tolerance of 0.005in.  In the programming we do set the tolerance to be 0.005, but I don't know if that overrides the post. Regardless is it possible to reduce the number of decimal places and change the tolerance?

Thanks!

[Anonymous]

Hey Bob,

I believe I had mentioned this before, but we have had some problem with data starving on our machine while running fusion 360. We looked at the G code from Fusion and from our old program and we noticed that there is an extra digit being generated in fusion. Instead of for example 0.001 it is generating as 0.0015. The machine is only accurate to within 0.005 so this extra digit is insignificant to us. My initial thought is that this is adding extra precision that is causing the machine to lag. I then looked at the most recent post we received and found under capabilities and tolerances that the tolerance is set to spatial (0.002,MM) if this is setting the tolerance at 0.002mm that is well beyond the precision we can achieve. Would it be possible for you to update the tolerance section to reflect a machining tolerance of 0.005 inches. In the programming we do set the tolerance to be 0.005, but I don't know if that overrides the post. Furthermore, in our old program it seemed that it was possible to generate whole integers without decimals and in fusion it appears it is not.  Regardless is it possible to reduce the number of decimal places and reduce the tolerance? 

On a side note, from your experience does this seem like it would reduce the data starving and lag we are experiencing?

Thanks!

[bob.schultz]

Hello Cameron,

The changes you are requesting are quite simple and something you can do yourself.  You already know what tolerance you want to set so just change the tolerance line.  It is also straight forward to change the number of decimals output and whether a decimal point should be forced with the axis register.

tolerance = spatial(0.005, IN);
...
var xyzFormat = createFormat({decimals:(unit == MM ? 3 : 3), forceDecimal:false});

  As far as I recall the tolerance setting is only used when linearizing circular records (outputting them as linear motion).

Data starvation is caused by a move finishing quicker than the control can read a block.  It was common with older controls and not so common anymore.  The typical fix for this problem is to set a minimum amount of time that each block must take to process, which will slow down the feed rate on blocks that would finish quicker than this preset time.  The easiest way to see if your problem is actually data starvation is to slow down the feed rate for the entire operation and see if you are still getting lag time.  In this case code can be added to automatically slow down the feed rates when necessary.

Another solution may be to increase the tolerance value in Fusion so that it does not generate so many points close together.

[Anonymous]

Hey Bob,

Just had a bit of a breakthrough with the data lag problem we have been having and I wanted to get your opinion and see if you could help us update our post to reflect the changes we need. Below is a recap of our issue for reference.

1) Our machine is experiencing a lag only while using fusion 360 programs

2) The lines of code generated by fusion are double that of our old software for the same program. (45000 for fusion vs 20000 for our old software)

3) This increase in code we know to be the bottle neck causing the data lag

By turning on radial command from fusion (allowing circular planes) we are able to get roughly the same number of lines of code as from our old software (20000 to 22000).  The only problem is it seems the post is not outputting our radial commands properly. The machine gets an error and displays the error "PGP: Insufficient data in the programming of a circle" for a line "N33 G03 X22.141 Z-0.085 R0.006 F150". From what I have determined the reason for this error is that the post did not specify a Y coordinate and thus there was insufficient data for the programming of a circle. When I output a code from our old software it post out G02 and G03 radial command and the machine reads them no problem, but it always specifies an x y and z before the r command (see below).

FUSION 360

N33 G03 X22.141 Z-0.085 R0.006 F150.

OLD SOFTWARE

N33 G3 X70.709 Y4.179 Z-0.125 R0.003

Is it possible for you to update our post to follow this format of xyz than a r command? I am attaching two programs below with radial commands, one from fusion and one from our old software as reference.

Thanks again for everything!

[scottmoyse]

---

@Anonymous wrote:

Is it possible for you to update our post to follow this format of xyz than a r command? I am attaching two programs below with radial commands, one from fusion and one from our old software as reference.

Thanks again for everything!

---

It's possible for you to contact a post developer and pay some money to get what is a very specific post sorted for you. There are a list of companies here. You've scored big time so far. Also if you go through your post yourself, you could probably quite quickly find where you need to force a Y axis output for arcs.

[bob.schultz]

Cameron, you can add the following commands in the onCircular function to force out the XY locations on every circular block.

---

@Anonymous wrote:

Hey Bob,

Just had a bit of a breakthrough with the data lag problem we have been having and I wanted to get your opinion and see if you could help us update our post to reflect the changes we need. Below is a recap of our issue for reference.

1) Our machine is experiencing a lag only while using fusion 360 programs

2) The lines of code generated by fusion are double that of our old software for the same program. (45000 for fusion vs 20000 for our old software)

3) This increase in code we know to be the bottle neck causing the data lag

By turning on radial command from fusion (allowing circular planes) we are able to get roughly the same number of lines of code as from our old software (20000 to 22000).  The only problem is it seems the post is not outputting our radial commands properly. The machine gets an error and displays the error "PGP: Insufficient data in the programming of a circle" for a line "N33 G03 X22.141 Z-0.085 R0.006 F150". From what I have determined the reason for this error is that the post did not specify a Y coordinate and thus there was insufficient data for the programming of a circle. When I output a code from our old software it post out G02 and G03 radial command and the machine reads them no problem, but it always specifies an x y and z before the r command (see below).

FUSION 360

N33 G03 X22.141 Z-0.085 R0.006 F150.

OLD SOFTWARE

N33 G3 X70.709 Y4.179 Z-0.125 R0.003

Is it possible for you to update our post to follow this format of xyz than a r command? I am attaching two programs below with radial commands, one from fusion and one from our old software as reference.

Thanks again for everything!

---

Cameron, you can add the following commands in the onCircular function to force out the XY locations on every circular block.

   xOutput.reset();

   yOutput.reset();

[Anonymous]

Hey Bob,

Just recently we started getting an error again saying "PGP insufficient programming of a circle" on programs that we had previously sent out with no issue. I was wondering if a fusion update has changed the way it is interfacing with our post causing an error in the g code. Below I am attaching a copy of the post, a f3d file that caused an error, and the corresponding g code that caused the error. Do you see anything that would be causing this error? It occurred in the second operation.

Thanks

[bob.schultz]

Hello Cameron,

The second operation contains helical entry moves, which apparently your control does not like.  You can add the following code to the top of the onCircular function so that helical moves are output as a series of linear moves.

  if (isHelical()) {
    linearize(tolerance);
    return;
  }

[joenbassman]

 Hi Bob,

We too have a routech 220 (from 1998) and were curious if you think that the resolved post would work well with our machine, which uses NUM 1060 rather than NUM 1080.

Perhaps we should save you the trouble and contact one of the recommended coders to write us a custom post for our machine.

Thanks for the help!

Joe

[bob.schultz]

Hello Joe,

Sorry, I cannot say if the post will work on your machine with the NUM 1060 control.  The best thing is for you to download and tryout the post.  You can then see if the output matches your machine's requirements.  If it does, then great.  If it is close you have the option of making the modifications yourself and/or by asking for support in this Forum.  If it is far off, then yes the best solution would probably be to contact a reseller that specializes in post processor modifications.

Thanks,

Bob

[scottmoyse]

Hi Joe,

With the SCM machines it's not so much about which control is used really. But if you are running Xilog Plus or not. But Bob's suggestion of just trying the post anyway is where you need to start. If you want to pay for post mods, then I'd be happy to look at it for you and give you a quote.

[joenbassman]

Thank you for doing most of the heavy lifting on the already existing post; I'll give it a cautious shot and see how it goes. My expertise in code is quite lacking, but I'm learning, albeit very slowly.

[joenbassman]

---

@scottmoyse wrote:
Hi Joe,

With the SCM machines it's not so much about which control is used really. But if you are running Xilog Plus or not. But Bob's suggestion of just trying the post anyway is where you need to start. If you want to pay for post mods, then I'd be happy to look at it for you and give you a quote.

---

---

@scottmoyse wrote:
Hi Joe,

With the SCM machines it's not so much about which control is used really. But if you are running Xilog Plus or not. But Bob's suggestion of just trying the post anyway is where you need to start. If you want to pay for post mods, then I'd be happy to look at it for you and give you a quote.

---

Hi Scott,

I'm still waiting on a new compressor to run the pnuematic tool changer on our SCM 1080. 

Could you give me a rough idea on what programing work to modify the post would cost? I don't know how things are going to go, but if we need to have some modifications done, I would like to budget for it.

@Please, feel free to email me @ lumberjackwoodproducts@gmail.com .

Joe