Multiaxis CircleMill toolpath question

[kool]

for Master cam X7,

 

Is there a way to out put multi axis circle mill tool path as arc ( I , j , k or r ) instead of xy xy xy and turn cutter comp on/off ?

 

Thanks in advance,

Kul

 

 

[Eric@HorsepowerInc.]

I asked our reseller this exact question a few times, over a few releases. Basically no, but if we keep asking maybe!??? Don't hold your breath.

[A.MAHLER]

That is handled in the post, it won't work with multiaxis cuts. you have to create a plane in Mastercam and use the 2d circmill in that plane. You can only output G02 and G03 in TOP, RIGHT or LEFT, FRONT or BACK planes unless your machine supports the creation of new planes but the setup for your post would very complex.

[mcpgmr]

I have cimco working on this for our DMU 50 post. I don't want I, J, K but just cutter comp g41 and g42. I was told the same thing about planes. We are close to having this working the way I want it.  One would think this is possible since Mastercam gives us the option in Multi Axis Toolpaths.

[mcpgmr]

So I'm curious, Has anyone been sucsessful at using Circle 5 Axis and if so what does your g code look like?

[MIL-TFP-41]

I gave up on circle 5 axis when I found out it linearized the arcs. Whats even worse, I never did find a setting for the tolerance it used to linearize. Till it works like regular circle mill, its just one of those things that is there but is never gonna get used.

[mcpgmr]

I hear you. I really want it to work. Saves time. Don't have to create a work plane and a operation for every stinking hole, Maybe this has been addressed in X8 and we can live happily ever after? 

[Guest MTB Technical Services]

Has anyone tried using the FBM hole milling functionality for this?

 

I used FBM at a customer site for 5-axis drilling of several hundred holes that were not normal to the part surface.

It worked perfectly and did it in just a few seconds.

 

FBM creates workplanes for each hole it drills/mills so this may be a work-around for those who really want 5-Axis Circle Mill with arcs.

[mcpgmr]

I want to try this FBM. Can you set it to ignore all features but holes a certain size?

[Guest MTB Technical Services]

I want to try this FBM. Can you set it to ignore all features but holes a certain size?

 

Yes.

[Guest]

I found earlier this year, comp on/off is broken on the 5-Axis circle mill. I reported this and was sent a bug/defect number.bi have not checked if it was fixed in X8 yet.

[mcpgmr]

Please let me know what you find out. Thanks!

[mcpgmr]

Wow! It worked like a charm! I got g2 and g3 plus cutter comp to boot! Thanks Tim! I did struggle at first because I tried FBM Mill. Have to use FBM Drill and disable any pre drilling of the hole if you don't want it. Thanks again!

[Guest MTB Technical Services]

Wow! It worked like a charm! I got g2 and g3 plus cutter comp to boot! Thanks Tim! I did struggle at first because I tried FBM Mill. Have to use FBM Drill and disable any pre drilling of the hole if you don't want it. Thanks again!

 

FBM for Hole Machining is one of the best kept 'secrets' in Mastercam.

 

What is inexplicable to me is why there is essentially zero promotion or documentation of the features and application of FBM.

It truly is an area where Mastercam has a distinct advantage above many of the players in the market.

 

It would be great to see Colin and eApprentice do some webinars or videos on the application of FBM.

[mcpgmr]

I may have spoke too soon. I'm not getting any arc in or arc out in back plot. Not sure I trust that the machine is going to apply CDC or if it's going to alarm out.

[mcpgmr]

I meant to attach these files to the last post.

[Rstewart]

Think you may need to check the start at center box.

[Guest MTB Technical Services]

It looks like a problem with the lead-in/lead-out because of the percentages for each.

You should try using start at center.

[Rstewart]

^^^^^

Beat ya to it lol

[mcpgmr]

Nothing changes when I check that box.

[mcpgmr]

Also, I would like to force it to use a tool of a certain diameter and no matter how I configure the chack boxes it still has a mind of it's own and selects a tool much smaller than what I would use. The hole is Ø.266 and I use a Ø.1875 e.m. FBM wants to use a Ø.125 e.m.

[Guest MTB Technical Services]

You need to tell FBM to only select tools within the part file and not to create them.

Also, tighten up on the selection range.

 

You can force it to do what you want.

[mcpgmr]

Must be bugs. I tried that. I even created a library with one tool in it and pointed the software to that library and it still creates a Ø.125 e.m.

[mcpgmr]

Here is the error I get and a snap shot of the parameters being used.

[mcpgmr]

Oh and I have one tool defined and that is a 3/116 e.m.