How to deal with no path when the slot to be milled is the same width as the tool bit.

[Inspections_JCH]

I am using an X-Carve to cut 2D profiles in 6mm plywood. I am using a 1/8" bit and would like to cut a 1/8" slot. In one of my previous designs I was able to do this when the machine thought I was doing the outside perimeter profile of the component.  But when I create a new design where all  I am cutting are straight lines the same width as the router bit it throws an error. Widening the slot fixes it. Using a 1/16" bit is not desirable.

The file is available if that is the only way to find the issue, but this really boils down to one question. "How to cut a slot the same width as the tool?"

[daniel_lyall]

Take .0001 of the tool size, have you tried traces or project?

[Inspections_JCH]

Thanks @daniel_lyall, I tried several .0001 and it finally worked when I got to about 0.25 wide. But why?  And no, I have not tried Trace because it is looking for a curve, and this component has no curves. I will see if AD has any tutorials on Project, but I am unsure that can be done with one line. And now I do not see project in the Manufacturing module. Could you point me towards it?

[Fabbunny69]

HI @Inspections_JCH 

Are you selecting the whole closed slot profile or just one longitudinal edge of the slot?

[Anonymous]

@Inspections_JCH 

It is a SLOT so you might be better be using the 2D Slot toolpath, this toolpath will allow the same size tool as the slot, see image and attached file.

Using the Slot toolpath will also allow you to set a "Move away" distance so the cutter backs away from the end of the slot on the last pass so that the cutter doesn`t "drag" up the end on Retract so avoiding possible finish/splintering issues, just run the simulation on the attached file and you will see how it works!!

[Inspections_JCH]

I have tried the slot. And the difference between the slot and the 2D Contour is that I was unable to add tabs at the bottom. That makes me think that the slot is intended for machining methods that will never use tabs. But to your point, the slot did work for creating a path that is the same width as the tool bit, and was rather easy to use.

[Inspections_JCH]

No, I only selected on line at the bottom. I will try to select the entire 'slot' as you suggest.

[DarthBane55]

What he meant is, make your endmill 0.1249" diameter, not go bigger.  Make your tool 0.1249 and it will work.  This software just doesn't like tools to be exact size as the slot for some obscur reason, hopefully one day they fix this because it makes zero sense.

[Anonymous]

@Inspections_JCH 

Reason for your issue is probably that you are doing something that no one ever thought of, slotting with the same size tool as the slot but with tabs is not something I have come across in years of CNC machining, I have done it many times on old manual Mills, real easy there, perhaps the Autodesk folks will pick this one up and run it by the developers.

Meantime, workaround, it is still easy to use the SLOT toolpath to do what you want, you will need to Model your Tabs into the slot and then use the Pattern function to copy them to all your slots, I have just done the one slot as an example, image #1 with modeled tabs will give you #2, just do two SLOT Toolpaths with different selections as in the attached file, very quick and easy to do once you get the idea.

@DarthBane55 

With respect

SLOT is the operative word here, this toolpat WILL allow the use of same size tool and slot, no need to mess around with altering tool diameters or slot widths, it works fine, right toolpath for the right job is usually the best way to go

[DarthBane55]

With respect, if he puts his tool at 0.1249 and uses 2d contour, he can then do his tabs without having to model them.  Sometimes using the "wrong" toolpath is easier and gets the job done.  I was just trying to help him out, he can do whatever he wants, and you as well, there are often more than 1 way to solve an issue.  Same end result.

[Inspections_JCH]

Thanks, I though the method I would use was to make the slot wider than the
tool which did not work. That would seem to be more like the real world
where we accept the tool as it is and then accept the results we get from
that tool. 🙂

[DarthBane55]

Strange, making the slot wider should have worked too. 

But, in reality, you should pick just 1 wall of the slot with 2d contour, don't pick the entire profile (that is fine if you use the slotting path as another user suggested).  If you pick only 1 side of your slot, your 0.125" tool will work with no regards to the actual slot width.

[Inspections_JCH]

I am happy to see multiple methods here. It gives me a better understanding of the capabilties of each method. These are learning exercises for me so trying each methods will serve me to develop my skills with Fusion 360.

[DarthBane55]

Exactly!  I would never say "my way is the way".  There are many ways to skin a cat, need to be a bit creative sometimes, but end result is what matters.  Enjoy!

[Inspections_JCH]

I believe that selecting one side is how I began this journey. But I never got a tool path so this was the puzzle.

I will go back and try this over to see if I can produce a file that you may be able to see what is happening.

[Anonymous]

With slot being same width as tool diameter, you only select one edge in Trace and 2D Contour, end fillets are impression of tool itself.

If you set any lead in and lead out values, it violates the model, really not rocket science, if you get an error, experiment to figure out what caused it.

You can do Slot, Trace or 2D Contour, each having some requirement that must be fulfilled in the way it's meant to work. If you must have tabs, that narrows it down to 2D Contour, if you skin the cat in every way possible, kill it first.

[Inspections_JCH]

@Anonymous  I tried Trace but it said there were no curves in my selected profile to use. Does Trace not work with straight lines? And I appreciate knowing that each method has requirements that must be followed. I will re-read each of the entries in the product documentation to see what I learn there. But I have read them before I started this journey and perhaps some of the details of the requirements went over my head. 😁

[Anonymous]

@Inspections_JCH 

IMHO The simple Contour toolpth that has been put forward by @DarthBane55  and @Anonymous would be the best option for what you want to do, what I put forward works fine but does require a lot more work as was kindly pointed out, yep, "kill the cat first before skinning" would be the quote of the day for sure.

See images, simple one sided Contour and the ability to set Tabs.

First image shows selection of edge in Model, second image is the toolpath with Tabs set and third image is Simulation of that toolpath. File attached

[Anonymous]

In my sample file, I picked same model edge in Trace as in 2D contour, I set tool compensation to left which puts tool to middle of slot in Trace.

If you want to drive center of the tool in Trace, you have to draw a sketch line in the middle of slot and select it as geometry in operation along with tool on center selection.

[Inspections_JCH]

@AnonymousThank you very much for your examples in the file that you attached. Your modeling of the slot was very different than mine. I created my slot by sketching a rectangle and extruding it.

Your examples in the manufacture module are also quite different. I will try to employ your methods in both design and manufacturing and see how it comes out for me. Perhaps my issues are more related to the design than anything else.