CREATING THREAD MILL TOOLS IN X8

[CADCAM3D5AXIS]

I have looked thru the topics on this and have been trying to get x8 to see the file , level, model, and every other way the topics say you can do and i must be missing a lot since i can not get the tool manager to see the tool as a file or even import from level that the tool sits on. i have even tried modifying tools to get the geo and that does not work for me anyways. if some one has a step by step for X8 to add a tool to the data base that the simulator sees i would appreciate it very Much. i get this error from the tool manager when i try to open or import the geo for the tool.

Thanks In Advance

i have spent some time on this with reading utube vids and the topics in emastercam going way back, so i am sure it must be 1 or 3 clicks away from being good for the simulator.

i do get the program to do my threads and the code is good  but i would like to see it so i can make other special tools that need to be drawn up and used in the simulator.

Thanks To All who have some time or info to get me were i would like to go for this issue. Also on the file import its looking for a DXF file but when i saved and created the geo there never was a selection for file format or geo format at least i did not see it.

 

 

 

[CJep]

Are you using an MCX file or level to define the custom tool geom?

Is the custom profile made up of lines & arcs - no splines?

Is the custom profile geom the only thing on that level?

Is the geom in the upper right hand quadrant?

Is the profile defined as an open contour?

[CADCAM3D5AXIS]

I AM USING A LEVEL IN THE FILE OF THE JOB I AM DOING

also using only lines no arcs

i have only geo on the one level and the dims on another

the geo has a centerline down the middle and only half the geo of the tool

I believe it is a open contour

 

 

.

 

 

does the color matter ???

TIA

[CJep]

If you have it defined as a center line no,

You also have extended the line on both ends, not necessary, but it doesn't hurt you either

So yes that would be considered an open contour

 

Is the open contour a continuous chain?

No duplicate or overlapping entities?

All the geom was drawn at Z zero in the TOP tool & construction plane?

Is the tool profile draw to scale?

How did you define the tool?

Did you select the "defined tool" that best describes the shape (I use a slotmill when defining threadmills)

[CADCAM3D5AXIS]

yes one chain with 7 total entities

no dups, or overlaps

drawn at z zero  in top tool and construction plane

drawn to scale  to the numbers of the tool ?

[CJep]

drawn to scale  to the numbers of the tool ?

 

Yes you can chose to draw it as the actual size or "scale" the tool up the way we created defined tools in the past (it would be drawn on size then scale to be 2.0 dia, then brought in as a defined tool)

 

You didn't say if you are using "?" as a custom tool or a "defined" tool (endmill, bullmill, facemill, slotmill are considered defined tools)

Some of the toolpaths require that you use a "defined" tool to be comped correctly, the multiaxis toolpaths require the custom geom to be run as a "defined" tool.

[Colin Gilchrist]

Can you put a file up with just the tool geometry? I can create a short video walking you through the process...

[Guest]

There's a custom tool video at my blog, check out New England CAM link in my sig , go to the Blog Entries

[Guest]

OK, it appears my hosting service is having issues with their Linux servers...here is the Youtube video

 

[CADCAM3D5AXIS]

Ok Guys

Thanks for the Input 

Here is a file with the tool in it with the op    i use it on .

Thanks CJep,  Colin, & John   for your Help   As always it is Very Much Appreciated .

You Guys   Are The Library Of Congress For Mastercam , and a list of other Very Useful things .

THREAD MILL TOOL SAMPLE TEST-1.mcx-8

 

Thank You All

Happy TGIF 

 

:cheers:

CADCAM

[Guest]

Very strange.....

 

I was getting the error as you.......

 

Finally, I did a save some and only saved the threadmill geometry to a file..........I tried making a new tool in a new file and was able to use the saved geometry in the file

 

Then I found your issue

 

You have blanked entities on the same level with the tool profile geometry, delete the blanked entities it will work fine...there can be nothing else on the level, not even hidden or blanked

[CADCAM3D5AXIS]

Thanks John

i got blanked ! 

i will check this out i just watched your utube vid   pretty straight forward .i will begin making some tools.  question does it make any diffrence how many teeth you draw for the single point thread mill or does it only matter in the tool settings in mcam?  and what do i need to change to get a thread mill with multi teeth to work in the simulator does this have to be drawn or not ?

Thanks

CADCAM

[Guest]

Thanks John

i got blanked ! 

i will check this out i just watched your utube vid   pretty straight forward .i will begin making some tools.  question does it make any diffrence how many teeth you draw for the single point thread mill or does it only matter in the tool settings in mcam?  and what do i need to change to get a thread mill with multi teeth to work in the simulator does this have to be drawn or not ?

Thanks

CADCAM

 

 

If you have a multi tooth threadmill, I have always defined them as such more for verification than anything else, as long as you define the number of teeth in the path you will get the appropriate path based on those numbers

[CADCAM3D5AXIS]

I just ran the updated tool and i have it saved as a special tool. it looks right but when i run the sim, it does not make any threads in the part in the sim. is there some other settings i should make or check? or set.

Thanks again

I shall mess with it some more in the am  bright and early.

:cheers:

Thanks Again

[Colin Gilchrist]

What did you chain for geometry? If you chained the inner circle (ID), you will have to use the Overcut amount to cause the tool to cut into the bore diameter.

[CADCAM3D5AXIS]

^^  +10000^^^^ Colin that did the trick  i have the thread geo represented in the mach,sim to match my part.  Question      with the overcut is it always the case to use the overcut on all thread tools ID  Or OD and is this setting always necessary to get the right connection between the sim, gui and the program ? and should it always = the pitch amount for thread depth  or is there anything else that has effect on the GUI or the software in general that may cause a hiccup ?  Also the depth of thread in the settings, this amount if you want to go to the bottom of a hole this depth is from the bottom of the tool  and not the center line of the cutting tool ?

Such as wanting threads to go all the way down but not hit the bottom can i just stay off the bottom by .005 or .010 and not have to worry ?? or can the start finish of the thread be control by the geo so you can get max thread depth?

  Thanks to all who Respond to this Thread with very useful Techniques and vids  they all are very Much Appreciated

:cheers:  

CADCAM

[Guest]

Typically, when I chain for ID/OD threads, I always have a diameter that represents the Major(ID) or Minor(OD)

 

and the depth is to the bottom of your tool, I have gone into holes .005" from the bottom

[CADCAM3D5AXIS]

Good Morning JP   

If you go as you say, can you use the allowance over cut to compensate for plating or tough materials  and leave the MAJ MIN   id od set to the correct Dia,s and still only change the overcut number so you do not have to change the Geo to get good threads ? just in case you are using the geo for some other hole feature ??

TIA

[Guest]

Generally at that point, it is left to the operator to use cutter comp and bring it into to final size.

 

We do use pre-plating gages, so I'll program to nominal and leave the final adjustments

[xycnc]

I could be totally in the wrong, but I always like programing mine with points instead of circle geo. I find it easier to be able to input the diameter that I want and if I import the thread file program on another job (mostly for NPT's) I find it easier. Like I said but I could be totally wrong. Just throwing it out there as an option.

[Guest]

I could be totally in the wrong, but I always like programing mine with points instead of circle geo. I find it easier to be able to input the diameter that I want and if I import the thread file program on another job (mostly for NPT's) I find it easier. Like I said but I could be totally wrong. Just throwing it out there as an option.

 

 

It's an option, no doubt.

 

I prefer the circle because in using circle mill and helix bore, I can multiple sizes in 1 tool path......I suppose my use of thread milling just grew from that same usage

[mig]

  Thank you JP for you videos

 It is very informative and well done

      Mike  

[Guest]

  Thank you JP for you videos

 It is very informative and well done

      Mike  

 You are welcome, I hope whoever watches them can take something away that perhaps the didn't know or quite understand

[CADCAM3D5AXIS]

JP   with the vids at least you have some info and visual tools to review if at some point in time you forgot or would like to share the info with newbees,  At least until it sinks into the grey matter you will not have to look at it to many times until it sticks.

Thanks for All the work on your part and others  who pay it forward, !  when they get the chance  since it is very handy info to have when needed.

 

 

Question  does it really matter what color the geo is when building it, and the help files also said you had to dimension the tool on another layer for it to work. Is that true ??

Thanks Again 

[CJep]

Question  does it really matter what color the geo is when building it, and the help files also said you had to dimension the tool on another layer for it to work. Is that true ??

Thanks Again

No, the geom color is not critical when defining mill custom tool profiles, when creating lathe tools it is.