Face - Dynamic Mill Help

[MIL-TFP-41]

What I was getting at was something like this:

That is a facemill. Not a high feed cutter.

Agreed my example was of a high feed cutter.

 

[David Conigliaro CNC Software Inc.]

[David Conigliaro CNC Software Inc.]

2 minutes ago, MIL-TFP-41 said:

What I was getting at was something like this:

That is a facemill. Not a high feed cutter.

Agreed my example was of a high feed cutter.

 

regardless, you used a sharp face mill with a custom profile, Mastercam never comps to the custom profile. At least define your face mill with a full radius and try to get it close to your actual tool profile. Here's your tool with a tweak. Look at the attached file, two good toolpaths with your tool tweaked and my highfeed, both correct. There are no problems here against facing.

 

dynamic face_DC.mcam

[David Conigliaro CNC Software Inc.]

Mastercam does what you ask. You asked it to use a sharp endmill shape and you loaded a different shaped tool at your machine. 

[David Conigliaro CNC Software Inc.]

Here's your original tool leaving material. You basically defined a flat endmill for toolpath compensation (yellow) and told Mastercam to use the custom profile (aqua) for backplot, verify and stock model as that would truly represent what will happen at your machine. Nothing is wrong here. Stock Model, verify, and your machine all show leftover material, that is correct.

 

[MIL-TFP-41]

I realize what you are saying. I get it. The problem I have with defining a facemill is illustrated right here

Do a contour toolpath with this tool and it drives it as a 2.94 diameter tool, when it clearly is a 3" diameter.

 

[JoshC]

sounds like you guys found a solution but i wanted to mention that a tool not accurately defined can cause this too. The last time i had this problem on one of our parts it was caused by me not fully defining the tool accurately, if your Corner rad of the Tool is not accurate then this could be the problem because a Flat end mill would use a different step over amount than a Bull end mill would.

[David Conigliaro CNC Software Inc.]

I can look into the face mill and Contour interaction.. 

[David Conigliaro CNC Software Inc.]

21 hours ago, JoshC said:

sounds like you guys found a solution but i wanted to mention that a tool not accurately defined can cause this too. The last time i had this problem on one of our parts it was caused by me not fully defining the tool accurately, if your Corner rad of the Tool is not accurate then this could be the problem because a Flat end mill would use a different step over amount than a Bull end mill would.

Thank you Josh, you stated my entire point of this thread. We must define tools accurately as Mastercam will intelligently apply them based on definition. Did you know...there are actually two very different processing logics behind Dynamic technology. One based on flat sharp endmills and one based on Bull nosed endmills. Ball cutters are simply treated like Flat sharp endmills. Using a Flat or a Bull can affect OptiRough processing time, there is more happening with Bull nosed to ensure no material islands or nubs are left behind...

[David Conigliaro CNC Software Inc.]

Some times, depending how you are using a tool, you must define it as two different tool types. For Example. I had this 3/4in all in one type tool. I could chamfer, spot drill and side mill with it. I used it to Spot drill in my part file at Tool #6. So I initially defined it as a Spot Drill tool type. Later, I was using our 2D Engrave toolpath and wanted to us it as an engraving tool as it could very well handle it.  The tool was already in the carousal and would do a good job. I selected it and received an error, no toolpath output. Engrave did not like the Spot Drill tool type. So I created an Engrave Tool type and assigned Tool #6. Yes, I received a duplicate tool # warning but I new what I was doing and Mastercam allowed me to define two Tool#6 tools that Mastercam would consume very differently even though it was the same single tool on my machine.

I was milling Aluminum billet Detroit Lions magnets!

 

 

[gcode]

One thing I've had trouble with is defining 90° face mills

If you define a Ø3" OD face mill with .06R corner fillets the tool's working diameter is Ø2.88

This is great for face millings as the face mill toolpath needs this info to calculate proper step over.

The problem arises when you use this face mill as an endmill on a computer /wear  comp contour tool path.

The system uses 2.88" as the cutting diameter and you get a .06" over cut and a scrap part.

We actually scrapped a part this way.

One programmer built a 90° face mill, used it for facing and saved it to the Master tool library

Months later a different programmer used this tool for some contour work and got burned.

The system needs to be able to use these tools as a face mill or an endmill and properly comp the working diameter.

As it is, it's just too risky to use a 90° face mill as we frequently use then as endmills also.

We just define them these tools as bull endmills to avoid this risk

 

see the attached file for an simple example of this issue

 

 

 

3 x 90 x 06r facemill.zip

[David Conigliaro CNC Software Inc.]

Yes gcode, I am currently discussing if we should be using secondary diameter for face mills in toolpaths other than facing with my Mill Team. Stay tuned. It's been this way for decades with very few complaints so it will be hard to get traction for fear of messing up regens in legacy files!

[Guest]

3 minutes ago, David Conigliaro CNC Software Inc. said:

It's been this way for decades with very few complaints

Not trying to be a smartass but has anyone been listening?

This has been an open and on-going issue, as you state for years.

Most people don't use it because it just doesn't work as it should

Edited November 1, 2017 by Guest

[gcode]

15 minutes ago, David Conigliaro CNC Software Inc. said:

It's been this way for decades with very few complaints

I'm guessing the reason there have been few complaints is because no one uses the 90° face mill definition

It's simply too dangerous to have  these tools in your library.

As a side note... I just tried to define this same tool in X6 and couldn't get it to work..

[David Conigliaro CNC Software Inc.]

 We also must way the impact of such changes. Changing a tool comp is very serious, massive impact, as it will destroy all existing files upon a regen in the version of Mastercam with the change. We have not received a high number of complaints on this comparatively speaking. But that doesn't mean a change is not justified, we just have to tread very lightly with tool comp changes.

[Guest]

1 minute ago, David Conigliaro CNC Software Inc. said:

, we just have to tread very lightly with tool comp changes.

On that I agree....that requires some finessing, no doubt

 

[gcode]

3 minutes ago, David Conigliaro CNC Software Inc. said:

 We also must way the impact of such changes. Changing a tool comp is very serious, massive impact, as it will destroy all existing files upon a regen in the version of Mastercam with the change. We have not received a high number of complaints on this comparatively speaking. But that doesn't mean a change is not justified, we just have to tread very lightly with tool comp changes.

I feel your pain... we have old legacy NC files here that defy all the rules of modern manufacturing.

We've been doing it wrong for so long it's too dangerous to do it right

As long as the old hands run the jobs all is well, but as soon as we put a new hire on it, its a forest of red tags.

[David Conigliaro CNC Software Inc.]

I'm sure you all already know this, but just reinforcing. Safest thing to do is define your Face Mill for facing as you get clean overlaps and such and define the same tool as a Flat or Bull nose endmill. As long as you use the same Tool# in Mastercam you can safely use the single face mill on the machine.

[David Conigliaro CNC Software Inc.]

5 minutes ago, gcode said:

I feel your pain... we have old legacy NC files here that defy all the rules of modern manufacturing.

We've been doing it wrong for so long it's too dangerous to do it right

As long as the old hands run the jobs all is well, but as soon as we put a new hire on it, its a forest of red tags.

Well said gCode, same thing goes for software development. It can be dangerous to change a legacy behavior affecting potentially 10's of 1000's of users. with 100's of 1000's of files out there.

[Leon82]

Now that I think about it there was a job where I need it to Dynamic face so I ended up making two facemills with the same tool number. The one I use for facing was .05 undersized on dia. And a full size one I use for my Contours

And then I told it don't make a tool change in the NCI.

[Matthew Hajicek - Singularity]

I never ever use the facemill tool type.  You can define an endmill with a chamfered corner.

Once people have adjusted their habits and workflow to deal with a problem you won't hear many complaints about the problem, but that doesn't mean it isn't a problem.

[David Conigliaro CNC Software Inc.]

On 10/31/2017 at 10:07 AM, MIL-TFP-41 said:

Ok, what if my 2" diameter facemill has a 1/4" radius? Use a bullmill?

You use a bull mill if you want to accurately comp the side of the tool, like in a Contour toolpath, yes.

[David Conigliaro CNC Software Inc.]

We have the 3 main generic tool shapes for 90% of work, Flat, Bull and Ball. Then we have special tool types like the Face mill, used for Facing blocks and also useful for chamfering the block after facing. Yes, the 2D Contour set to  'chamfer' on the cut parameter page will comp accurately to a Face mill with chamfers. Those two things make good sense for Face mills, other than that you have to go a different route using Flat, Bull or ball.

[David Conigliaro CNC Software Inc.]

It all boils down to understanding how your tools are consumed by toolpaths while realizing defining tools accurately is paramount. Hopefully you all see how we try to balance flexibility against not making the software too flexible which can introduce confusion. We don't want to go crazy adding all sorts of exceptions. A tool can't behave this way over here, that way over there, another way somewhere else. Hard to learn and teach. We chose to make Face Mill behave oneway relative to it's cutting diameter and gave it one exception by supporting the 2D Contour Chamfer toolpath recently as we felt there was good continuity there, facing blocks and cleaning up the edges go hand in hand.

[Newbeeee™]

47 minutes ago, Matthew Hajicek™ - Conventus said:

I never ever use the facemill tool type.  You can define an endmill with a chamfered corner.

Once people have adjusted their habits and workflow to deal with a problem you won't hear many complaints about the problem, but that doesn't mean it isn't a problem.

True - I've only ever used endmill and created a facemill of the right dia.

Can't remember why - could be because I always have, or because I read here about being burnt because we side cut using comp too.