[Scott_M]

Can I define a custom tool ?

The tool I need is a 90 deg double angle cutter . None of the "Tool types" in the tool manager will work properly. It is a side milling cutter and the slotmill is close but I need to define the geometry on the end.


Any help would be greatly appreciated


Thanks


Scott

[cadcam]

Yes you can best idea is to go pick the tool that is close and right click and edit tool. Now click on the ?mark and it will tell you about custom tools. If you get stuck let me know.

[Scott_M]

Hi CadCam

Thanks for your response ! I had tried that but it would not let me "Modify" to what I needed. I ended up modeling the tool and saving it as an mcx file and used the "?" undefined tool page . It looks Ok but It will not work as planned.

In the attached screen shot you can see the tool and what I am trying to cut. I have the "Tip Comp" set to center and it is still using the bottom ( Tip ). This is putting my cut way off the part. Also seen in screen shot.

And when I try to do the bottom angle......it does nothing ...except whine about "cutter comp unsuccessful" and gives no tool path.

At this point if I could even get it to do the top I would just edit the "G-Code" with an updated "Z" height for the bottom angle.


Or just tell it it is 2 different cutters , A chamfer mill for the top and a dovemill for the bottom. ( With the specs for my cutter of course )

I just thought it might be easier than this.

Any thoughts would be greatly appreciated !!!


Thanks


Scott

[cadcam]

Can you Share that file with me and the tool if it is in the file on another level.

[Scott_M]

Hi cadcam

thanks again !

I will dummy up another file with the appropriate geometry. I do not want to release that paticular file , some proprietary info is involved.


Where do I send the file ? I can not attach an .mcx file...or should I just rename it or zip it ?




Scott

[cadcam]

Hi cadcam

thanks again !

I will dummy up another file with the appropriate geometry. I do not want to release that paticular file , some proprietary info is involved.


Where do I send the file ? I can not attach an .mcx file...or should I just rename it or zip it ?




Scott

You can send me the MCX file you said X2 correct?
I have 5 version of X on my box just need to know so when I send it back you can open it up.

Send to "cadcam at Mastercam-cadcam.com"

[Scott_M]

Files sent

Thanks !!

Scott

[cadcam]

Files sent

Thanks !!

Scott

So you want this to happen correct.

[Scott_M]

Yes sir it is !

And on the other 3 faces of those 2 90 degree projections.


Scott

[cadcam]

Yes sir it is !

And on the other 3 faces of those 2 90 degree projections.


Scott

Scott the file I sent you was a XMR1 file and it had all the sides done using the solid to program with and your tool on a level instaed of a seprate file.

Cadcam

[cygnus x-1]

I have the "Tip Comp" set to center and it is still using the bottom ( Tip ). This is putting my cut way off the part. Also seen in screen shot.

Scott

Hi,

I just found this thread after searching and I'm trying to do almost exactly this same thing; except with a radius cutter instead of a double angle. I thought setting "tip comp" to "center" would compensate for the side radius, and it actually does when you verify the tool path. But when I post the operation it doesn't do the compensation. I can get the desired result by changing the depth of the contour manually but that seems like kind of a hack.

I have the tool defined as a slot mill with a radius. That part seems to be fine. It just won't do the Z compensation.

Oh, and I'm using X2 with a Haas 3-axis mill. Any thoughts?

Thanks!

[cadcam]

cygnus x-1 can you show a picture of the shape or share a file. the option for center of cutter is how to compansate say in 3d contour use the center of the spher instead of the Tip of the tool.

[cygnus x-1]

cygnus x-1 can you show a picture of the shape or share a file. the option for center of cutter is how to compansate say in 3d contour use the center of the spher instead of the Tip of the tool.

Ugh, just now getting back to this. I figured out how to do what I needed to do but I'm still confused about what tip comp does. So it sounds like tip comp only applies with 3D contours?

Here is a file with the part I was working on:

http://bluegreenlabs.com/Misc/TipComp.MCX

There are two tool paths in the file. They both produce the same shape when the tool paths are verified but they produce different G code when posted. With either of these operations toggling tip comp does nothing to the posted code.

Chris

[Superman]

Generally, "Tip Comp" is how you are going to set the tool-length in the machine, and mastercam will give the code according to that tool setting method.
99.99% of the time, you would only use "TIP" comp. "Centre" would be for a special occasion
AND also note
----tools CANNOT have mixed "tip comps" if using the same tool length #.

Imagine a ballnose cutter
-if toolpath set to "Centre", imagine the path of this point to go over a semi-circle, starts on the c-line, moves over the top to the end, the setpoint will be going thru an arc----mastercam would output arcs
-if toolpath is set to "Tip", going over the same semi-circle, tool tip point starts 1/2 the radius below the c-line, travels to touch the top apex, and down to be a mirror of the start point, the setpoint is moving in an ellipse---mastercam would output point to point.

now compare the actual tool movements to each other, they are identical
and they create the 1/2 circle form - 2 different g-codes, 2 different tool setting methods

[cygnus x-1]

Generally, "Tip Comp" is how you are going to set the tool-length in the machine, and mastercam will give the code according to that tool setting method.
99.99% of the time, you would only use "TIP" comp. "Centre" would be for a special occasion
AND also note
----tools CANNOT have mixed "tip comps" if using the same tool length #.

Uhh, hmm. When you say "...how you are going to set the tool-length in the machine..."; does that mean if you want to use "centre" tip comp with a ball nose mill you would have to set the offset *in the machine* to the center of the ball? If that's the case then it would explain what's going on with the form cutters as well. I would need to set the offset to the center of the radius on the cutter and not the end (in the machine).

Yes, I think I understand now. This would also explain some strangeness I was seeing on another 3D surface job. I think I had tip comp set to center when it should have been tip. From what I've noticed the tool path parameters always seem to default to "centre" tip comp though, which is annoying if it should really be "tip" most of the time.

Very good then. I'll go play some more and see how it goes. Thanks for the help!

C|

[Superman]

Why not pre-set all your ops to common settings ?
( you know, get rid of tthe "Tip Centre" setting, set the tool comp to "Wear" , lead in/out to 10% [ don't set a value- it take a % of tool dia ], set gouge check on etc.)

> Goto the operation manager.
> under the "machine" , go "Settings"
> in the lower part, you have ops and defaults
> open the defaults file
this blanks out your geometry screen and opens a "mini-operation" screen that list all your available strategies, even the surface paths
> select the 2D_Contour operation and go into it's parameters, do your pre-setting here, including on all contour types ( don't forget the "Ramp" and even the "Ramp options", uncheck the "Linealise Helixs", turn ON "Final pass at depth" ) etc
> back out, accepting as you go