Do you see anything wrong?

[Rotary Ninja]

Ok. Lets try this another way to test some things out.

 

I will create three different 3/4" threadmills. The first will be drawn on-size as MCM does.

 

The second one I will draw on-size as well, but lets assume it has a 1" shank for some odd reason. This tool is just a test because I want to try and figure out how Mastercam pics up it's compensation.

 

And this last tool was drawn on-size then scaled to 1" at the point I will be using in the tool's parameters to define it's diameter.

 

All three of these will work depending on how you define them in the tool's parameters.

 

Here is MCM's undefined tool drawn to size. It works just fine.

 

 

Here it is using a Slot mill instead of an undefined tool. This does not work.

 

Here is the large shank tool using an undefined tool. The shank is drawn at a 1/2" radius. This for some reason does not work. The tool's tip radius as you saw is drawn at .375", just like the first tool. The tool is setup to be .750" diameter at this same point. But I guess since the shank is the larger point Mastercam tries to use that to display the tool (just guessing here).

 

And here is the large shank tool using a Slot mill. I have no idea why this works, but it does.

 

Here is a tool drawn at 1" scale using an undefined tool This does not work.

[Rotary Ninja]

And here is the way I draw all of my tools. This is a tool drawn so the radius is at 1" and using a Slot mill instead of an undefined tool.

 

This not only works in this case, but it also works if I want to use this same custom tool profile but set it up as a 1/4" threadmill in the tool's parameters.

 

This does not work for the unscaled tool.

 

It also does not work for any of the other tools in any other configuration. Only the tool scaled to 1" can be used for multiple tool diameters. All you have to do is change the diameter to the appropriate size in the tool's parameters. This is the reason I do this. I don't have to draw 25 different port tools.

[romeo123400]

I agree, I have never had to scale the tool either, just draw the tool to its radial dimension and it should output an exact cutter.

Maybe the scaling affects sizing the tool within the tool params page for different size cutters.

 

 

Great job on the pics Rotary Ninja HHHoooooooooooooooooooowwwaaaaaaaaa

[MoMo1108]

very well put together and i do it the same as ninja only i use it on a layer in the program so its allways with that file

[Mic6]

I draw tool exactly as it sits on my desk(radius), use a dashed red center line. Save to custom tools folder. Create new tool>undefined>custom file>cutter diameter is the actual cutting diameter. Back plots/verifies perfectly. Pretty cool how there are so many different ways though.

[djstedman]

I don't know if it helps anyone but if anyone wondered and is interested..

 

The reason to scale it to a 1 inch diameter is simply based on math..

 

Anything drawn with a 1 inch diameter can be easily scaled by multiplying any size given as 'diameter' on the tool info page..

 

For example,

If you specify its .25 diameter .25 x 1 = .25

If you specify its 5 inch diameter 5 x 1 = 5

 

This allows you to draw one single point threadmill tool as shown above.. and scale it for use over and over again any time you need to use that type of tool..

 

If you draw it to scale it will only work at the one and only size you drew it at.. scaling will not work and will be totally messed up.. because..

 

If you drew it .5 diameter and you specify its .25 you would have mastercam internally do the math as .5 x .25 = .125 which isn't correct..

 

I haven't done extensive testing of this to prove it out.. but as someone that used to do a lot of computer programming in the past it seems logical that this is the reasoning..

 

All that being said.. as with a lot of things in Mastercam the ability to draw scalable tool is really cool.. and in a lot of places very useful, on the other hand most likely a complex one off port tool would have absolutely no reason to be scaled.. so IMO its a matter of knowing whats available and using the best option for your given situation

[Alumenium]

When ever i have tried to make a new tool using Rotary Ninjas method,

as soon as i pick the file ive drawn, i get an error saying something wrong with the file or data

even went step by step and drew RN's tool as show in this thread

whats that about? any ideas?

[Rotary Ninja]

Make sure everything is trimmed correctly. I have had this happen a few times. I just redraw the tool and it usually solves the problem if trimming doesn't fix it.

[Colin Gilchrist]

I've got a comment regarding the 1" scaling issue.

 

If you use a normal tool type like flat, ball, bull, slot, ect., you can draw a custom profile shape, and Mastercam will automatically scale the tool when you enter a different diameter in the define tool dialog.

 

Using an "undefined" tool (which really should just say "custom" in my opinion), Mastercam will not scale the profile for you. You need to draw the tool profile to size (still only draw half the tool from centerline), and the diameter you enter in the diameter field is what Mastercam will use as the defined diameter for offsetting from the geometry. Think about a contour toolpath, set to 'computer' compensation. This radial offset will be calculated from the diameter you enter when you define the tool.

[Alumenium]

all the trimming is good , but still the error

[Colin Gilchrist]

Can you post a picture of the tool geometry you've drawn please?

[Alumenium]

Gladly

 

thank you

[GF8er]

Gladly

 

thank you

 

delete the center line

[Colin Gilchrist]

Also, delete the dimension if it is on the same level as the custom profile. You should only have the outside profile of half the tool, with no centerline. (Mastercam assumes the Y axis is the centerline)

[Newbeeee™]

Neat job Ninja

[Alumenium]

Yeah, deleting that stuff did not work, only comes back with new error "improper argument"

[Rotary Ninja]

If you post the MCX file I will take a look at it.

[Rotary Ninja]

I've got a comment regarding the 1" scaling issue.

 

If you use a normal tool type like flat, ball, bull, slot, etc., you can draw a custom profile shape, and Mastercam will automatically scale the tool when you enter a different diameter in the define tool dialog.

 

Using an "undefined" tool (which really should just say "custom" in my opinion), Mastercam will not scale the profile for you. You need to draw the tool profile to size (still only draw half the tool from centerline), and the diameter you enter in the diameter field is what Mastercam will use as the defined diameter for offsetting from the geometry. Think about a contour toolpath, set to 'computer' compensation. This radial offset will be calculated from the diameter you enter when you define the tool.

 

Ahh. That makes sense now.

 

Also, delete the dimension if it is on the same level as the custom profile. You should only have the outside profile of half the tool, with no centerline. (Mastercam assumes the Y axis is the centerline)

 

If these are not supposed to be there why are they on the tools that come with Mastercam?

[Alumenium]

Ok, Thanks RN

TAPE 2 THD MILL.MCX-5

[CJep]

There are multiple issues with the tool geom, the "center line" is not a center line Mcam sees the geom as being a closed boundary and the tool origin is incorrect.

[CJep]

I was able to get McamX5 to load and comp the tool correctly defined as a slotmill, using the dia and flute height as drawn. The tool geom would not draw correctly in the lower right of the tool definition utility. If you try to adjust the size of the tool in the tool definition the dia will comp but remember the flute height is being scaled accordingly. The custom tool geom is on level 100 of the part file.

[Rotary Ninja]

I was at work trying to post a reply but was too busy with a setup. I tried moving the tool to the origin and changed the centerline to a dashed line and this still didn't work. I ended up redrawing it to get it to work, but we have X6 anyway. Did you have to change any other geometry?

[Alumenium]

This is the first time ive noticed Origin mentioned. is it supposed to be center bottom of tool? or where

[CJep]

Yes, bottom center of the tool profile.

 

If you are going to use the geom as defined you could bring it in as a lolipop tool. If you are wanting to bring it in as a slotting type tool then the geom needs to change. If you are wanting to able to adjust the size of the tool as needed then you will need to define the tool the same as Kevin "the Rotary Ninja" described for you.

[Rotary Ninja]

This is the first time ive noticed Origin mentioned. is it supposed to be center bottom of tool? or where

 

Sorry, I probably should have mentioned that. I always start by drawing a center line to represent the center of the tool from the origin straight up in Y. Then I draw a line from the origin across in X to represent the bottom of the tool. I offset these lines to draw my tool. Then I trim everything up and connect the dots to create the angles and such. Then I scale the drawing so the cutting edge is 1" as shown. I have never tried, but I assume if you were drawing a port tool for instance, and you wanted to touch off the spot face portion of the tool to set your Z you could draw the tool with the port section below the centerline. Brb