Printable View
I am machining some silicone molds and when I generate the toolpaths, the toolpath shows that it is under the surface. You can only see it if you turn the part to wireframe. However it only does this in the bottom of the channel not the sides. Attached are photos of molded parts. You can see that the bottom is thicker than the sides, also it is chamfering the edge of the mold which is leaving the pointed part on the edges. Any thoughts or ideas?
What version of MasterCam? Post the file you are working with and/or some screen shots.
I am running Mastercam X3. I will post some screen shots of the toolpaths so you can see what Im talking about.
Here is the toolpath shown in solid and wireframe. Since this is a surface toolpath operation Mastercam shouldnt machine any deeper than the surface right?
there are many factors that could cause the tool path to be below the surface. can you attach a file with just the problem tool path so others can look at it and offer suggestions?Quote:
Originally Posted by moto1965
Here is the problem toolpath. Its machining fine on the sides but 0.002" deep in the bottom of the cavity.
i see what you mean. i was not able to get the tool path to not violate the faces you want to machine on your solid model and i could not find anything wrong with what you did. i converted your solid model to surfaces and it seems to machine the surfaces without violating them like it was doing with the solid. have you tried doing the same to see if it works for you? i tested your solid part and mastercam says the solid is good.Quote:
Originally Posted by moto1965
I have not tried that, I will try that on the next part I make and see if it fixes my problems. It may just be the way the designers are creating the surfaces in solidworks. Thank you for your help, ill post what happens.
can you try it on this part to see if converting the solid to surfaces is what you want? i would attach my file but you are using x3 and i am using x5. here is a screen capture. if this is what you want i wonder why i can not get a good result on the solid but only on surfaces?Quote:
Originally Posted by moto1965
What happens when you change Tip Comp to Center and adjust machine offsets appropriately?
i can try that on his file. why should this make a difference?Quote:
Originally Posted by txcncman
Since he is using the side of the radius of the ball mill to machine the sides, the tip of the tool is pushed deeper into the part to make contact at those points. I do not know for sure this method will work, that is why I posed it as a question, not an answer. See screen shots.
i asked because i do not know when i should use tip comp or when i should use center comp. i am still not sure when i need to change to center comp. maybe depends on the cutter? guess i have been lucky as i always use tip and have not had a problem. want to know more. i am here to learn and help where i can.Quote:
Originally Posted by txcncman
How did you convert the solid to surfaces? I guess I dont know how to do that.
Quote:
Originally Posted by moto1965
menu:create;surface;from solid
The actual problem is... there is no problem
the shade setting of the actual solid,
you have your setting at .0020", if you set it to the same as your cut tolerance of 0.0005", then the toolpath has NOT violated any of the solid
Screen --> Shade Settings --> Chordal Height
a coarse setting is good for general screening of most parts, making the resolution finer does use more PC resources AND slow the system down considerably
I see what your saying with the shade settings, that makes sense. Do you have any ideas why the part would come out the way it did in the initial post? You can see from the molded parts that the bottom is thicker than the sides. I have noticed this on a few molds I have made but some clients don't care about a 0.002" difference but some do.
i changed the setting to .0005 and i still have the same problem. you looking at backplot in wireframe like i am?Quote:
Originally Posted by Superman
The graphical representation of the solid ( that you see on the screen) is just that.Quote:
Originally Posted by moto1965
The toolpath uses the solid with the "System Tolerances" ( in system config --> Tolerances) to generate the initial path offsets, then it applies the operation's tolerances to put the paths on-screen, it will then ( if your settings allow it) apply a smoothing &/or an arc tolerance to shorten the NC code
solids are drawn using this chordal setting, but surfaces seem to be shown correctly....as Tx has demonstrated
try a 0.00005" settingQuote:
Originally Posted by Joesph Jackman
when Verifying, set the tool tolerance to .0005" to see a more accurate "representation" of the finished part......hope you have a bit of spare time as it will take a while
The tolerance setting ( in each operation ) is the critical one to set to get correct paths, the solid chordal setting has no bearing on toolpath calculation.
I finally determined what the problem was...eroded tool probe. My Renishaw tool probe had actually eroded away or actually developed a dent/crater in the middle of it. The dent was so small I couldn't see it without looking at it under a magnifying glass. So the problem was large ball endmills (0.125") would probe fine because the tip was large enough not to go down in the dent but when I would probe a small ball endmill (0.010" or 0.020") the endmill would go down into this dent and the machine would record the length. But the actual length was a little bit longer by however far it went into the dent. I hope this makes sense and everyone should take a look at their probe anvil to make sure it doesnt have any issues.