Best approach to machining multiples?

[JetForMe]

I looked around a bit but didn't find an obvious result.

What's the best way to make several of a part? I've modeled the part in F360, done the CAM for it, and made one. But I'd like to step-and-repeat the operation a few times, as my stock is large enough to accommodate several. I've been doing it manually, by re-zeroing the machine to the right, and re-running the gcode. But I wonder if there's a better way. I don't really want to make multiple copies of the body in F360.

This is on a Tormach PCNC1100, if that helps with the answer. But I'm hoping I can do it in F360 CAM, by specifying the stock size and, and being able to simulate the results.

Thanks.

[LibertyMachine]

Pattern is your friend. The screen cast below shows with 4 models on screen, but there is an option for distance:

[CGPM]

How many tools are you using to make the part?  Subroutines and multiple work offsets are how I do it to keep the amount of code to a minimum but I haven't tried doing this in Fusion yet. 

[j9lemmon]

Is Patterning still the best way to cut multiple copies of the same part? 

Just wondering if anything has changed since 2016.

[DarthBane55]

Depends, if you don't want a WCS for each part, yes for sure.  If you need a WCS for each part, no it is not.

In the setup, post process tab, there is an option for multiple WCS offsets.  This will output the code with each part having its own WCS.  Limitation here is that all parts must be in the same orientation, because the code is just repeated exactly in an identical manner for each instance.  Or you can use G68 between parts if they are not orientated the same way.

[j9lemmon]

Thanks @DarthBane55 

So, if I want all parts in the same orientation,  I use Patterning to duplicate the parts and set the distance between each part, and I make NO changes in the Post Process Tab of Setup? Is that correct?

[DarthBane55]

With pattern, the parts can be in any orientation you like.  Just use "component" pattern, you will see that it will create the toolpaths for each instances of your part (you need to place the parts in your file), no matter orientation.  Limitation: they will all be using the same WCS origin.

With the post process tab multiple WCS offsets, you won't see the paths on screen, they will only be in the posted code (if I recall correctly), and each part will have its own WCS.  Limitation:  parts must be in the same orientation (unless you can use G68).

Hope it clarifies.

[j9lemmon]

Yes, @DarthBane55  this does clarify. Thanks!

[DarthBane55]

It would be so great if component pattern would allow for a WCS for each instance!!  That would solve many issues in 1 go!

[j9lemmon]

I'm trying to learn how to using the Post Process tab of Setup in Manufacture, following your suggestion about WCS, @DarthBane55 .

The Post Process failed after I guessed at values for the fields in the Post Process tab. Any thoughts? A screenshot:

[seth.madore]

@j9lemmon  could you share your file? What machine and post processor are you working with?
If your initial G5x is set to 2, that would give us an initial of G55. You have it set to two instances with an increment of 14. Is this intended? That would give you a G55 and a G54.1 P10. If you're getting an error, it's possible that you're not setup (in your post) to use G54.1Pxx values

[j9lemmon]

My Machine is the Millright CNC Carve King. I do not use a WCS system. In Manufacture - Setup, I normally choose Model for Orientation. 
I don’t know G code, so I’m afraid a can’t answer the question about G54. 

[seth.madore]

When you input a value of "14", what was the expected result?

[j9lemmon]

Since I had never used the Post Process tab of Setup, I entered 14 because I want each copy of the part to be 14 mm apart. Obviously that was incorrect.

Is there a step by step tutorial about using the Post Process tab of Setup in Manufacture?

Thanks for any advice.

[seth.madore]

Ah! 

So, since you don't utilize work offsets at your machine, and the desire is to have two sets of toolpaths spaces 14mm apart, the best solution is to CTRL+Select all appropriate toolpaths, right click and select "Add to new Pattern". Set Pattern type to "Linear" and define the spacing to suit.

 

[j9lemmon]

Thanks! @seth.madore 

Sounds ideal for my situation.

So does this mean I don't even have to duplicate the model in Design? I just create on model in Design and then go to Manufacture to do the steps you suggest?

Thanks again.

[seth.madore]

Yep. ONLY downside is that you will lack proper toolpath simulation, since the second instance of the model doesn't exist, only the toolpaths. But, that's a minor issue

[j9lemmon]

I put your suggestion to work @seth.madore 

It worked perfectly, except:

I expected to cut 4 parts, but after cutting those 4, it started to cut another 4 roughly 100mm away from the 1st 4. Here's how I set up the Linear Pattern: 

• 2 instances in one direction
• 2 instance in the 2nd direction
• I checked Keep Original
• I chose Order by Operation
• in the Post Process tab of Linear Pattern, I left Override WCS unchecked

I tried about 5 variations, changing the values of the Linear Pattern, but keep getting the same result.

Any advice?

[seth.madore]

Hmm. Share your latest file if you can. What post processor are you using?

File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply