Issues with part setup tutorial

[Merik Karman]

Hi

Just getting back into the pocketNC after an absence.

I am trying to follow the "part setup" tutorial and I have a question, I apologise if it is a stupid one.

I open the Vice and table as instructed. I thought it would be better inserted into a current empty design but I am trying to follow exactly. I then insert the cube and dismiss the movement options.

The tutorial then says to move the two gripper set screws. I select them and then try to move them 20mm in the X. They move off in the wrong direction. For my setup I have to move them in the Y.

This is not major but clearly I have missed some step or got the environment wrong.

I would like to get the tutorial working with a common frame of axis at least :-)

Any help would be appreciated.

Thanks

Merik

[Randy Kopf]

Merik:

Good morning. I would not get too hung up on the verbiage... You can see where they need to end up. It's likely that somewhere in the order of the things you did that it sees directions differently.

I saw a couple things that were off as well but just try to do the overall concepts.

In my case I moved the part a little higher above the vise as a couple other people here have had issues with the tool getting really close to the vise.

When I got into the tool paths for that part I did not care for the method of controlling the cut motions. So I sketched my own boundaries.

Consider that tutorial good to show how to import models and how to set up parts and deal with different cuts on different faces. But use caution on actually cutting a real part.

When I get off work I can upload my part model to show how I controlled the tool path..

Randy

[Merik Karman]

Thanks Randy

I will crack on and try not to get too concerned about exact matches. If you could post your files that would be greatly appreciated.

Thanks  Merik

[Merik Karman]

OK So I went through all of the setup tutorial and generated GCODE and ran it without a tool.

It is so wrong! The spindle tried to drive through the bottom of the B axis table sideways (IE table flat and spindle flat)

So I clearly have a miss match of some sort with axis.

There was no interlock or limit switch to prevent this, so I assume I have not got something setup correctly.

MK

[Pocket NC]

Merik,

If you send your Fusion file to us at in...@pocketnc.com, we will take a look at it and let you know what's going on!

[Merik Karman]

Randy

Thanks so much for this. It all works for an air cut so far and looks good.

Do you have any other example files that are a little more complex that you are happy to share?

Once again thanks so much.

Regards

Merik

[Merik Karman]

I spoke to soon. The last issue I have is how to place the vice on the table so it matches the model in Fusion.

During one of the cuts the spindle body still comes into contact with one of the black vice set screws.

My belief is that maybe I have the vice in the wrong position on the machine.

Is there an easy way to know / reference the correct position on the machine for the vice.

Once again thanks

[Randy Kopf]

Hi Merik:

I have a couple other files that I posted out earlier that might be of help jump to this post to see those...

https://groups.google.com/forum/#!topic/pocket-nc/anfiQrBirvU

I have a couple other files in the works but I'm not quite ready to post them just yet. One is simpler that I made reference to in another post about Tool Length Offsets.

https://groups.google.com/forum/#!topic/pocket-nc/zhDmkSP-lPw

And the other part I am doing for the Pocket NC is a bit more complex. It is a 5 AXIS ARTIFACT. And that is a model that is used to test cuts, and then do measurements. My ARTIFACT model addresses 2 Axis through 5 Axis machining aspects. And it has a focus on the Pocket NC. I also have a part with some 3D contouring but it's not 4 or 5 Axis just 3D Milling. Some of the other files I have were done with Desk Proto so they won't help you unless you had that running. 

:-)

Randy Kopf

http://desktopartisan.blogspot.com/

[Merik Karman]

I do have desk proto multi axis edition and also Vectric Vcarve Pro. The latter is mainly used on my CNC router.

[Randy Kopf]

Merik:

Give me about 1 hour and I'll post a graphic showing the full machine, the vise orientation and the part.

If you are getting close to the set screws something is not right... So just hang loose a bit.

And I'll also post a Tool Library that includes both the Old Spindle and New Spindle that you can add as a holder to your tool. That will give you an added sense of what is going on.

Randy

[Merik Karman]

Thanks.

I couldn't find support for PocketNC inside Desk Proto? Do you have a configuration to suite?

Regards

Merik

[Randy Kopf]

Merik:

I just updated the math on this part. What I discovered was there were collisions with the bottom of the spindle and the top of the vise. I am looking for set screws issues but missing something?

My updated Fusion 360 CAM model is located here:

https://drive.google.com/open?id=0BxziiLimgn9SeGNoNjVGV3M2LWc

I deleted the earlier post I made, I concede there were errors. And I update new links here in this post.

Just be cautious as we are human. I know I am missed the target, but hopefully this will get it just a little bit closer.

Here is what I discovered tonight.

1) The Pocket+NC+Test+CUBE math is challenged with respect the the Y Axis heights proposed.

2) I shortened the Cube Part height from 1.000" to 0.75" to limit the PNC Spindle VS Vise clearance.

3) I added the Pocket NC spindles as Fusion importable Tool Library Holder Models both Old Spindle and the New Spindle. 

The link to the spindle as holder model file is 

https://drive.google.com/open?id=0BxziiLimgn9SaExNSlFoVDZZNWM

4) I ran tool path checks against both spindles as tool holders and saw collisions on both version of spindles on the prior math I uploaded. 

5) By altering the math to 0.75" Part Height there is no longer any risk of either spindle coming close to the vise.

6) I added a static model of the published Pocket NC kinematics. I broke the link to this model so it can be included for a start position only VS Vise position placement only. That model is not displayed to avoid visual distraction. This model is NOT a dynamic simulation model. Other CAM systems like Unigraphics support full dynamic machine simulations as Tokyo Pav has been at work on. Mastercam also support this 7) The new spindle is 16.77mm diameter VS the old spindle is 27mm diameter. The new spindle has 5mm additional clearance above the vise. If you have the new spindle you could make the Test+Cube part 5mm taller.

8) I am uploading both old and new spindles as PDF's

https://drive.google.com/open?id=0BxziiLimgn9SbGNrWVExSURoVWM

https://drive.google.com/open?id=0BxziiLimgn9SeVNvMm4telF3Ulk

And Fusion 360 Models

https://drive.google.com/open?id=0BxziiLimgn9SWTlRdGhQUE5PMWM

https://drive.google.com/open?id=0BxziiLimgn9SU3p3QnFhUlhzemc

Randy

The graphic below is a snapshot of the attached model. Everything I mention is included.

[Merik Karman]

Thanks a lot Randy. Would it be possible to get that post you deleted back, it had a lot more info in it that was very useful.

I am running another air cut now.

I am currently on the old spindle but my new spindle shipped today from the USA on its long trip to Australia.

Thanks

MK

[Randy Kopf]

Merik:

Regarding DeskProto and Pocket NC...

So early on the folks at Pocket NC were considering DeskProto as a bundled solution. They ran into some issues with the way DeskProto is configured. And DeskProto was CAM only requiring a CAD front end. About this time Autodesk came along and offered Fusion 360 as a more complete CAD/CAM solution. The folks at Pocket NC did not complete the development of a DeskProto Postprocessor. Now I personally do 5-Axis machining at my day job www.rmbproducts.com. I've done multi-axis machining with UGII, Pro/NC and now Mastercam 5-Axis. So I was influenced by another Pocket NC user to look at Desk Proto. You can see in other posts or on my blog that I was fortunate to have Gary Swank a veteran Desk Proto user for 10+years to engage me. Gary is interested in the Pocket NC. If your in Portland Oregon proximity connect with Gary in person. So Gary assisted me in getting Desk Proto running on the Pocket NC. I am open to offering the Post(s) that were created from this effort. But prior to doing that it is very important to understand the pro's and con's to running DeskProto on the Pocket NC. 

So one major fact is DeskProto is a creative pseudo multi axis software. It does not do full 4 Axis machining, It must always point it's Z Axis at the center of rotation and does not support off position 4X machining like CAM Followers. It does do a fantastic job of contstant rotary machining of about an axis along a contour. So it does bust and most rings etc. It does not do full 5 Axis machining in fact it only does a strange variant of 4 Axis with psuedo projected 5th Axis mode. But it does some really clever things and what it does do it does extremely well and it does extremely fast. Delving into the nuances of DeskProto is it's multi-axis version supports a primary rotary axis by default as an A-Axis. The problem with this is Pocket NC made a really strange choice to make it's only full 360 rotation table to be it's B-Axis. So that is the conflict of weirdness here getting Deskproto to say A and Pocket NC to hear B. So the Pocket NC selected the B Axis as as primary and A-Axis as partial to go along with a design that could sit on a desk with a minimum footprint

So the DeskProto team simply re-maps the output code to fake using the A Axis and output it as B-Axis code. But even with this there is some issues in setting up the part models in DeskProto.

That is enough for now,

:-)

Randy

[Randy Kopf]

Merik:

 

Here is the earlier post information... Without the link to the prior outdated Fusion 360 CAM Model as the prior version had a potential for collision.

 

Earlier post starts now...

 

So the part I am going to load is my take on the Pocket+NC+Test+CUBE.

the original tutorial is here at http://www.pocketnc.com/part-setup

 

But my version does a few additional things.

 

1) It adds another part model to constrain tool path... to what we really want to cut.

2) It shifts the part 1/8" up in Z away from the nasty vise set screws.

3) It includes NC Tool paths that made into NC Patterns to automate the cuts on each side.

4) Cutting the part:

-4.1) It cuts the TOP but since the part was moved up in Z by 1/8" it only makes 2 passes downward.

-4.2) It cuts the let side of the part with the TIP of the cutter and stays away +.050" per side. (Color coded with RED Surfaces.) 

-4.3) It uses a NC Pattern to replicate that left tool path on to each additional cube side.

-4.3) It cuts around the upper portion of the part with the SIDE of the cutter to 1.000" finish size 

(The surfaces color coded with GREEN Surfaces.)

-4.4) A manual operation is inserted M0 (VERIFY OD's MATCH CALIBRATE TOOL LENGTH)

This is a natural place to pause the program and do some measurements.

5) MO STOP - AKA TIME TO MEASURE YOUR PART!!!

The TOP width of the part shown with green surfaces should measure 1.000" wide.

And the LOWER part shown with RED surfaces should measure 1.100" wide (0.050" Stock Allowance)

 

If the lower portion is off by any amount, then your tool length is off.

I.e. The lower portion measure 1.080" and should be 1.100" that means the tool cut 0.010" deeper with the TIP than it should have. The Pocket NC thinks everything is fine.... But the fact is it cut 0.010" deeper. So just stop the program and RESET your tool length. What we know is Pocket NC does not realize that your tool is 0.010" longer than it thinks it is. that is the ERROR. so tell it that it is longer. 

 

6) Recalculate your tool length offset

 

OLD SPINDLE CALC:

3.600 - TLO - ERROR = ADJUSTED TOOL LENGTH.

3.600 - 1.000" - 0.010" = 2.590"

 

NEW SPINDLE CALC = I don't have this to really now how to deal with it...

 

Other things to consider:

There are two spindle types plays a factor. I am also machining my Pocket+NC+Test+CUBE with Freeman Wax. It is much more suited for cut and measure scenarios. This material is easily obtainable off eBay or Amazon or other sources via Google search like Otto Frei or Rio Grande.

 

DISCLAIMER: I'M NOT RESPONSIBLE IF ANYONE CRASHES THEIR MACHINE USING MY INFORMATION. Had to say it... 

 

Just take it slow everyone.... Like set you rapid and feeds down to minimal possible.

 

Screencast showing the essence of what I did... The audio sucks sorry???

https://knowledge.autodesk.com/community/screencast/e49a0f47-3efe-4b73-ab92-98d40cb56098

Additional detailed screencast that is a little garbled... But it mostly explains what I did that is different.

https://knowledge.autodesk.com/community/screencast/9ee13e77-c457-4344-99e5-bdf0ffb67e95

 

 

Randy Kopf

http://desktopartisan.blogspot.com/

[Merik Karman]

Randy

I have done everything that you suggest including reading up on tool lengths etc.

I ran your program with no tool or stock and everything ran perfectly.

I then had to modify your file to change two things so as to reflect my tooling and stock:

1) Changed the stock size; and

2) Altered the tool to a 4mm 2 flute end mill.

The modified file is here : Fusion3D File

The Tool Library is here: Tool Library

My machine looks like this with stock and tool loaded and the machine homed:

When I run the program I get an error about linear move on line 15629 would exceed joint 2's positive limit.

The Error I get is:

The machine looks like this at the time it throws the error:

I have included the NC file here: NC File

I am very grateful for all the help you have given and sorry that I keep bugging you. I have tried to include as much info as possible.

Once again thanks.

Regards

Merik

[Merik Karman]

I forgot to show the image of the tool table.

[Randy Kopf]

Merik:

Your machine is identical to mine. 

The virtual setup of vise orientation and actual material is correct. 

What is wrong is the CAM Setup. The stock model is wrong in your file. The values are way off.

I think because your stock is so much taller your running out of Y Axis stroke. 

See my graphic and try to adjust your stock to match.

Also make sure your using the 1/8" supplied single flute Harvey Tool as T10. The value in the Tool Length Offset page looks close in range. BTW all values in that table should be - negative numbers. Your T4 has a positive number. Not that it is in effect or anything.

I'll try cutting an actual part using my program in the morning.

Also the line number in the program you mention does not exist.

No bother BTW in helping you or anyone. This is complicated stuff and you seem to be doing very well with it!!

:-)

Randy

[Merik Karman]

The stock looks right to me. You can see from the images is seems about correct.

I am not using the 1/8 cutter, I am using a 4mm cutter and it is tool 1.

I made the changes (I thought) to all the NC operations and regenerated all the toolpaths.

I included the tool library to show you.

The version of the F3D file I included in the post has all the stock and toolpath updates.

Regards

Merik

[Randy Kopf]

Merik:

Good morning. The actual stock looks great. I see a difference in your CAM Setup. 

And the stock defined in that is different. 

I think is making at least 4 more passes above your part than mine.

I thought it be causing the axis stroke limit?

Randy

  

I see a difference in each of our parts above the part itself.

[Randy Kopf]

Merik:

I am stepping through this problem with you. It's normal to do this to eliminate possible errors. Your stroke limit may be a combination of things.

The next question is about your Tool 1

How far does it stick out of your spindle?

Lets step through what I see...

The Tool table input you have is -0.984"

The Old Spindle Calculation is 

-[3.600-StickOut]=Input Value

Using algebra 

3.600-Input Value=StickOut

-3.600-0.984=2.616

It tells me your tool must stick out 2.616" from the spindle?

When I look at your photo and compare the stock height as roughly 1.5"

And look at the tool in your spindle it does not look like it sticks out of the spindle the same amount.

It looks shorter like maybe it sticks out just under 1"?

Is it possible your input should be -2.616" with and that your tool actually Sticks Out only 0.984"?

Randy

[Randy Kopf]

Merik:

I output your program without any changes to my Pocket NC

I used the supplied Harvey Tool with an Tool Table Input of -2.489" for T1

I did not load the physical cutter just to play it safe.

But your program ran complete without any issues.

Here is the file...Output Ran on Pocket NC from Merik's CAM File

That tells me your only issue is getting the Tool Length value correct.

Randy

[Merik Karman]

Randy

Thanks again, I only just woke up on this side of the planet. I will try your theory at the machine later today and let you know.

At least I think I now understand the tool length calculation.

Regards

Merik

[Merik Karman]

With regard Deskproto, the only reason I am keen to get it working with PocketNC is simple workflow from STL parts to subtractive machining.

While I would love to reach out in the Portland area, I am 7,817 Miles away in Australia :-)

[Merik Karman]

Hi Randy

I sorted the tool length and ran the entire program through. It all worked fine.

I am cutting Acetol (Delrin) with a 4mm 2 flute end mill and that is where the next problem starts.

The tool stalled and everything stopped. I think you mentioned that this file of yours was setup to machine wax?

I now have to try and sort out new speeds and feeds and passes to suit the harder plastic and eventually aluminium and brass.

MK

[Merik Karman]

The tool I am using is SKW WF880 4mm 2 flute carbide cutter with 55 degree helix angle.

[Randy Kopf]

First did you determine the correct tool length by making actual cuts and measuring your part?

-

YES that file was set up for wax.

-

To machine hard plastic or even metal it's important to get the correct Surface Speed to base your feed and speed calculations.

-

But it's equally as critical to understand cut load. That was wax was using a radial step over of 50℅ of the tool diameter.

-

There is no way you will be able to do this with hard materials. There is an additional factor and that is total rigidity of the machine. Specifically the Pocket NC is a light duty machine. Another factor is having the right tool designed for a specific material. Companies like www.harveytool.com  provide extensive information on tool selection and starting feeds and speeds. Other companies like SGS Tool or Swiftcarb provide volumetric calculations too optimize depth of cut VS radial step over. And the calculations are not linear. That means both rpm and feed rate change based on depth of cut VS step over. Most advanced tool companies cutters are designed to cut with maximum flute length possible that is full depth of cut. However this last factor requires advanced tool paths that provide constant and smooth engagement. That means smooth lead ins and outs and gradual step over like morph spiral motion. Straight motions that reverse directions harshly like in corners are also serious problem for harder materials and a light duty machine. 

-

Else you have a crash and you will break tools or stall the spindle and jam your machine.

-

What this all means is you want a very small step over especially in harder materials.

-

The rpm and feed is not really going to change much since the cutters are so small in diameter.  As a baseline on a very rigid machine using carbide Aluminum has a SFPM of 1500. Brass is 900 

-

Again the big thing you want change is radial step over.

-

As as starting point I suggest the following:

-----------------------------------

Wax use 50℅ radial step over
Hard plastic 10℅ radial step over (0.4mm step over with your 4mm tool) 
Aluminum 5% radial step over (0.2mm step over with your 4mm tool) 
Brass 3% radial step over (0.12mm step over with your 4mm tool) 

One final thing to address is maximum rigidity for work holding and not sticking the tool out of the spindle any more than required. That means a flimsy held part and a really long tool will diminish your rigidity and negatively impact how well the machine will cut.

[Merik Karman]

Thanks again.

Clearly you can see I am a newbee to this CNC game :-)

I've looked in the Fusion NC tool path definitions and I can find step down but no reference to radial step over.

I assume that this is something I have to calculate and place elsewhere in the tool path definition? Or in the tool library?

Does that mean I should create 4 tool entries in the library? For example 4mm end mill Wax, 4mm end mill plastic, 4mm end mill aluminium and 4mm end mill brass? Each with appropriate speeds and feeds?

I haven't checked the tool length calibration yet because my first cube didn't go well. I stopped it before any damage.

Regards

Merik

[Merik Karman]

Hi Randy

I noticed your fantastic hold down options for the PocketNC on Desktop Artisans. Am I able to purchase this gear off you?

They look really amazing.

Regards

Merik

[Randy Kopf]

Merik:

The value you asked about is in each tool path definition screen... it is referred to as "Optimal Stepover" OR "Stepover". You can see it through each of the various tool paths creation screens.

.

YES if I were you I would definitely have 4 Machining Templates defined each as a starting points for each of tool paths based on you 4 variant materials:

1) WAX

2) HARD PLASTIC

3) ALUMINIUM

4) BRASS

5) Wait what, don't add a fifth material, at least not now!

As for KOPF tooling it is designed for a desktop machine and we have some of it available. Details to follow.

Randy Kopf

[Merik Karman]

Im feeling really silly. I have looked at your tool paths and none of them have stepover anywhere.

However I created a simple face operation as a test and it does have stepover mentioned in passes tab.

Is it something else in a 3D adaptive clearing?

Regards

Merik

[Randy Kopf]

Yeah don't feel silly. There are too many names for the same thing.

3D Adaptive mill calls it "Optimal Load"

2D Pocketing calls it "Maximum Stepover"

2D or Parallel calls it "Stepover"

And I mention these two because on shallow surfaces though you are stepping down in slices the nature is your stepping along a surface.

Ramp calls is maximum Stepdown.... 

Contour calls this Maximum Stepdown.

It is all the same thing.

You don't want ever cut with more than 50% of the diameter of the tool. Even facing you can leave cusps in acute areas.

And the info I gave last night says modern cutters are designed for cuts with the full length of flutes. The magic is in how much you step over...

Again this is a very light duty machine. I'ts not rigid and does not have the horsepower.

So or your first rough cut set "Optimal Load" to 0.4mm on that hard plastic.

 

[Merik Karman]

Got it cutting now, that is good.

I found that it wouldn't cut to the edge of my stock?? So I expanded the size of my stock by .2 inch.

No difference. Maybe the toolpath is being bounded by something?

There is a machining boundary selection, so I guess I need to expand its size a bit.

I can't find how to identify and expand the chain that is being used as the boundary selection.

But progress is being made. I think we should perhaps use parameters / variables for this so that we just go into "change parameter"

for a new stock or part size.

I assume that the best bet would be to have a starting file with most of the tooling and machine parts modeled with dummy stock and boundary selection all driven out of parameters.

MK

[Merik Karman]

Randy

What I am trying to do now without getting too confused is to create a starting point reference model.

I think that I want to try and get the tree cleaned up with components or groups.

Thinking a component or group for Stock

One for the machine and fixtures

One for the product that we are trying to make.

Trying to use parameters for things like stockX, stockY and stockZ.

Trying to use expressions like stockX + 1mm for toolpath containment for example.

Not sure if I can use parameters in CAM area for stock for example but should be able to based on choosing stock as a model.

Basically I want to try and capture all the good teachings / learning from this thread into a starting point model that is cleaned up and easy for anyone to start with, perhaps one metric and one imperial.

Then add a bunch of standard tools.

Then add the CAM setting for Wax, Plastic, Aluminium and Brass. You would then take the starting point model for the correct material, set the parameters for stock size, import your model and then go to it creating and/or modifying the included reference CAM configurations.

Do you think this is achievable?

Regards

Merik