Problem- Problem with Arcs

[mrcodewiz]

I have been having fits with the CAM side the last few days. I have been doing a lot of 3D modeling in Alibre, exporting to DXF, then importing those into Dolphin to create the CAM paths.

The problem I am having is that where one line fillets into another to create an arc, MACH3 ends up seeing a complete circle. So if I do a Goround on a profile, instead of following the line around it will try to do a full a360 around the corner.

The drawing looks fine and the simulation in partmaster cam looks fine. If i edit the geometry in cam it also looks fine. Its just in mach3.

Here is a drawing to help explain. Suppose I had a triangle created by 3 circles with tangent lines across the circles. If i do a goround, it will sometimes treat the fillet path as a full circle (the dashed circle in this picture) ane basically eat into the part.

It has something to do with the export/import. If I just create the part from scratch in Dolphin, I don't have this issue.

I hope that makes sense and someone has seen this before.

[mrcodewiz]

Here is an actual example that I just exported, added an NC profile, then post processed in CAM.

[andre-dolphin]

Hello,

I think the problem was with the post-processor - it had arcs being output as quadrants, not sure why this was.

I have attached a new job and a post that doesn't split arcs.

Also, just curious as to why you weren't using the Chamfer command, it calculates the offsets based on the angle of the tool.

ATB
Andre

[mrcodewiz]

I wondered if it was the post processor. I tried both of the 2 processors that I mainly use which are m_mach3_rotary and m_mach3_peck ( because one works well with the 4th axis and one works well with peck drilling). I didn't try the original one but I will start using that one unless I need to use the 4th.

I am not too familiar with editing the post processor files but maybe i'll try to compare them to see what the differences are?

As far as why I don't use the chamfering command, I guess I just got out of the habit of using it. My first machine was a little sieg X2 and it couldn't take very big cuts. If I wanted a .05 DOC and used the chamfer command, it just tried to take it all in one pass regardless of what I had the tool's cut depth set to which was too much for the poor little X2. I don't do it like this now but using a goround with a negative offset allowed me to chamfer and still have it recognize the tool's cut depth.

[mrcodewiz]

That post processor seems to work much better but for whatever reason, it wants to run the cutter down toward the table at the end of the program. It is incremental so I changed mach3 to use incremental mode instead of absolute but maybe I am missing something else? the whole program seemed to run fine until the end.

[mrcodewiz]

Is there a change I can make to my absolute PPR files that would have the same effect?

[John S.]

Can you post your code in zip format, so we can have a look at it.

I use this same post processor with no problems.

Are you using tool length offsets ?

John S.

[mrcodewiz]

I am not using tool offsets. I will create a sample and post it tonight. thank you.

[mrcodewiz]

Here is a sample I created. It is just a simple circle that I do a go round on. It seems to work fine but at the very end, it moves the Z to -1.2178 for some reason. I set both distance and IJ to incremental in mach3. Thanks for any help you can provide.

[John S.]

Late here so I'll have a look tomorrow but the code looks good, nothing in the code that will make it move to Z-1.2178.

Try running the same code with line 60 "M06 T11" edited out and do an air cut well clear of the work.

John S.

[mrcodewiz]

It looks like it is the G28 z0 command. If I zero my machine coordinates the same as my work coordinates it works fine.

I don't use my limits to home - just as safeties. In fact right now, I only have X and Y limits wired up even. So normally, I don't use machine coordinates for anything. I just leave Mach3 in non-machine coordinate mode (is this considered work coordinate?) and zero on my part before I start working. I guess I can switch to machine coordinates after I zero in and zero them all out as well but that seems weird. I guess I am supposed to set my machine coordinate Z0 at my limit switch and then the G28 would cause the Z axis to raise to my limit switch at the end of the job?


Can this post processor take the place of my peck drilling and rotary post processors?

[John S.]

Yes that post can do everything, peck and 4th axis.

Glad you found the difference with the co-ordinates.

Never thought to get you to check this as we don't use work and machine co-ordinates.
because the KX series mills are aimed at total beginners who can't get their heads round the two different co-ordinate systems we wrote a special screen that forced both systems to be Work Co-ordinates.
So the machine always goes to where you have specified the zero datum point.

John S.