Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Fusion 360 and Syntec 2 post processor for Laguna Smartshop M

6 REPLIES 6
Reply
Message 1 of 7
jason.chinchen
166 Views, 6 Replies

Fusion 360 and Syntec 2 post processor for Laguna Smartshop M

I have a new Laguna Smartshop M in the high school woodshop where I teach.

It has a Syntec controller and I am having some problems with the posts using the Syntec 2 post processor found in the Autodesk posts page.

 

My posts are all running about 9mm above the spoil board. I have touched off the tool, surfaced the spoil board and set the external shift, but still cant figure out why my contour cuts wont cut at the level of the spoil board as I have the machining set to do in Fusion.

I am assuming it has something to do with the first few lines of code that include the tool compensation commands but don't know enough G code to be able to decipher the issue. The other possibility is that a Z setting in the machine control software is wrong.

 

I will attach a fusion file and the post.

FUSION FILE:

https://a360.co/3Nyy1WL

 

 

6 REPLIES 6
Message 2 of 7
njdupreez
in reply to: jason.chinchen

The generated code roughly looks OK.

 

To check if your Z height is correct, jog the tool down so that it almost touches the spoilboard; Now the Z coordinate on your DRO should be almost 0.  If this is not the case, then most probably something is amiss with setting the Z=0 reference position i.e. "Adjusting External Shift".

 

Message 3 of 7

Please tell me where to find the }"DRO"?

I dont see any Z numbers at zero besides the G54.

Spoil board thickness is 17.73 mm-ish so that is what the external shift is set to.

Thanks.

Message 4 of 7

"DRO" means "digital readout", which refers to your controller display and it's XYZ position values.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 7
njdupreez
in reply to: jason.chinchen

What I mean is that when the tool that you'll be using to run the pass is jogged down to just above the spoil board, then your z-value, as circled below, should be zero (or very close).

njdupreez_0-1702940438581.png

 

Message 6 of 7

Is this the monitor screen?

Thanks

 

Message 7 of 7
njdupreez
in reply to: jason.chinchen

Yes.  I've taken the picture out of the manual for the SmartShop® M found at this link, Laguna SmartShop(R) M Manual, therefore yours might look different.

 

What you want to establish is whether your Z-axis's work offset is set correct for your stock and the program.  Your zero reference that you have chosen is the top of the spoil board (i.e. bottom of the stock).  This means that, having the tool loaded for the operation, when the tool's tip is just touching the spoil board, the machine's Z-axis value should be zero.

 

In the program that you've sent through in your initial post, you can see the following block:

 

N55 G43 Z21.59 H01

 

N55 means block number 55 and is basically just a line number.

 

G43 H01 together means to activate tool length offset (TLO) compensation number 1 (H01).  TLO compensation was disabled in block N10 with the G49 code which is normal practice.

 

Note that normally H01 refers to the TLO for tool number 1 and in your program you use tool number 2.  However it depends on the controller and possibly how Laguna has configured it but it might be the cause of the discrepancy.

 

Z21.59 means to move the controlled point (tip of the tool) so that it is at position Z=21.59 mm.

The value 21.59 (0.85" = 21.59 mm) comes from what you have put in for the "Length below toolholder" parameter in Fusion 360 when setting up the tool.

 

Note that"Length below toolholder" is related to the H01 number in your controller but it is unlikely to be numerically equal.  It all depends on what point the manufacturer used as the machine's controlled point.

The effect of this block is to just switch on tool compensation but keep the tool head physically in the same spot i.e. move numbers but not the tool head.

 

The block that follows N55 is:

 

N60 G00 Z7.35

 

N60 is the block number.

G00 Z7.35 means to move the machine rapidly downward (from 21.59) so that the Z position will read 7.35 on the DRO.  The number 7.35 mm comes from the stock thickness (1/4" = 6.35 mm) plus the "Safe Distance" parameter (0.0393701" = 1 mm) that is on the "Linking" tab of the "2D Contour 1" operation in Fusion 360.

 

Note that in the Fusion 360 file, on the "Heights" tab of the "2D Contour 1" operation your have the following parameters set / selected:

Feed Height: From = Top Height

Feed Height: Offset = 0 in

Top Height: From = Stock top

Top Height: Offset = 0 in

This means that your machine will run with rapid movements up to the point where it touches the stock.  This is not common practice because, due to set-up and machine tolerances, the tool might be run into the stock at rapid feeds.  It would be best to change the "Feed Height: Offset" parameter to something small like 0.1 " at least.  In this case though Fusion 360 prevents possible collision by raising the "Feed Height" so that the "Safe Distance" in the "Linking" tab is in effect.

 

The next block, shown below, starts the cutting:

N65 G01 Z0. F333.

N65 is the block number

G01 Z0 F333 means to move in a straight line (G01) to Z=0 position at a feed of 333 mm/min ("Plunge Feedrate" of 13.123 in/min set under the "Cutting Data" tab for tool 2).  This is the first line where the tool should be cutting stock and it cuts to the bottom of the stock.

 

In this block the machine is commanded to cut to a position of Z0 which is the top of your spoil board.  Therefore the axis data of your program is correct and the cause of discrepancy is probably one of the following:

  • Incorrect set-up of machine zero position for the Z axis
  • Tool length offset compensation

I hope that this provides enough background information to allow you to identify the cause of the error.

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums