Show Posts

This section allows you to view all posts made by this member. Note that you can only see posts made in areas you currently have access to.

Messages - sibianul

Pages: [1] 2 3 ... 19
I was limited to 5 attachments in my previous post, so here is the model I was playing above

...but for me neither would be a suitable workaround as there is a much simpler solution called Carbide create. It is able to build me a toolpath with two cutter sizes and automatically calculates where the big one missed and creates the path for the smaller tool aswell. Saddest part about Carbide Create is its totally free.

Hy, I just tried Carbide Create , for simple and big parts probably Carbide Create is great, but for complex and small parts, Carbide Create is just a joke :)

I played with it about 15 minutes, and found 2 serious issues (maybe there are some workarounds, but I haven't noticed any)

1. When defining tools there is no option for TOOL TIP DIAMETER

2. It seems the MAXIMUM RESOLUTION of Carbide Create is not high enough for small details, In my example I have some SMALL letters  (the smallest in this model is 1.3 x 1.5mm). If you check the toolpaths and also the imported DXF file, there are many straight lines instead of arcs, the toolpaths lines don't follow the contour of the letter.

So, Carbide Create is not usable for small parts.


Back, to CamBam now :)  yesterday and today I tried today to optimize even more my workflow, my main problem is that I'm losing time milling air, on the exterior regions of the models, on areas where I already milled using a flat end mill. I'm losing time because I use a very small 0.2mm tip  V-cutter, the feed is around 100mmpm and DOC is 0.1mm sometimes the Target depth goes to -1

While the REST MACHINING option is still missing, I tried 3 new strategies, hoping I can mill the parts faster.

1. I usually use the 2mm Flat Endmill to mill around letters, with an additional 0.2mm ROUGHING CLEARANCE , than I start milling with V-cutters, 1mm tip, 0.5mm tip and 0.2mm tip size, the last two operations beeing the most time consuming, as the feed is quite slow, around 100mmpm and a 0.1mm DOC.
Yesterday I had a new ideea to create an offset contour around the entire word to limit the AIR MILLING TIME, and it worked great, instead of 35 minutes now it mills the same thing in 27 minute, but it still mills AIR, as you can see in the photo attached, it mills on the interior of the new contour created and also on the exterior of the letters, until the toolpaths meet. It would be perfect if I could just use the same Slope Profile MOP but limit the area to the selected contour, like the BOUNDARY option of 3D profile MOP , this way it will mill on tight space, and on exterior sides where the material is already removed by flat endmill, will only make about 2 passes.

2. Then I wanted to try to mill using 3D Profile MOP because I knew this operation has the BOUNDARY feature that can help me save some time . If this option was available for normal 2D Profile MOP it would be a good alternative to rest machining, but still would need time to manually create shapes to avoid milling air, but less time than the COLISION DETECTOR plugin, which for detailed models  is very time consuming.
The problem with 3D Profile MOP is that it doesn't care about the TOOL PROFILE, when I used the same 30 degree V-Cutter, the toolpaths generated should look very similar with the above attached, Slope Profiles MOP's, but instead the toolpaths is exactly like it is would be when milling with flat endmill.

Probably an possible solution to this, is to model the solid surface, with the angled walls, instead the straight vertical walls, BUT I DON'T KNOW HOW TO DO IT IN CAMBAM, I can do it in Fusion360, but Fusion360 has his own issues with those imported DXF files.

Fun fact: Today I was laughing with my colleague because on one stamp I was working, it took a little bit more than expected for Cambam to generate the toolpaths, about 20 seconds , and while I was waiting my colleague seen me I was smiling/laughing alone, he asked me : What's Up ? I responded: I just imagined how Fusion360 would crash when trying to import this same model, that has a few thousands segments  ;D In cambam I just used the Arc fit option, and the time reduced to less than 5 seconds. In Fusion360, after many posts on their forum, the most common solution is : "You should try to redraw the entire sketch, in fusion, and not import that garbage dxf...."

3. Vcarve MOP. I tried this in the past and I noticed that on some small features, the model was overcut, I tried again now and the toolpaths looks ok but there still is something missing:

  • The DEPTH INCREMENT option is missing, and I don't think that the 0.2mm V-cutter will last to long when plunging in the Brass material, if anyone has any experience, please share it. I would try again, using the spindle RPM close to 20k , maybe this way it will work better.

Monday if the machine will be free of jobs, will try a sample with V-engrave plugin, to see if it will mill ok. I have some doubts, but will let you know after milling a test part.

So, long story short:
1. The 2D Profile MOP with the SIDE PROFILE option set to SLOPE, is great, but it's missing the BOUNDARY option!
2. 3D Profile MOP has the BOUNDARY option, but it doesn't care about the TOOL PROFILE I set, and it will overcut the model when milling with a V-Cutter.
3. V-Engrave it also looks good, but it's missing the DEPTH INCREMENT option, and option that all other MOP's have.

@tsikows, have you tried the COLLISION DETECTOR plugin?

It does work but you need to manually fine tune the generated lines.

Unfortunately I think I was one of very few people that needed this function, when working with Fusion360 I use this function on all my steel dies, without it the time needed to mill the steel parts would be much higher, as I mention when I opened the thread, for me this is quite important and I say it again, I would pay an UPGRADE FEE, let's say $50 - it would be ok for me, if this function would be available, and I'm sure others would agree to pay a fee for this upgrade.

Those lines are malformed because the underlying geometry has issues, this causes what you are seeing.
There is a companion plugin here that will clean and repair the geometry.
Just a short reply Dave as I'm quite busy :(, the lines are NOT malformed, are exactly how they should be, maybe I wasn't clear, it's just I had to draw the arcs to join OPEN lines toghether, because only when the lines are closed, Cambam could detect the collision when doing the slope profiles.

PS. I milled the part and it came out perfect :) I'm just posting the file to make things clear, maybe I wasn't clear enough in my previous message. I exploded the left corner so you see how the slope profile is milled if the lines are not closed. For simple models like this I will definitely use your plugin more often, even If I will have to manually join the lines together, it's more riskier on complex models, where there are many small unmilled corners .. but in time I will let you know how it goes. After this part that  milled yesterday, I'm quite happy, the plugin is very useful :)

Thank you Dave again !!!!

Today I used the plugin for the first time in an actual part, not just tests .. I'm sure I will use it more an more :)

I noticed on this model that if the polylines are open (the ones generated by your plugin) CamBam's internal collision detection functions don't work, and it's milling trough my model, but if I manually closed the polylines generated by your plugin cambam's collision detection works as expected :)

I like the troc mops too and have made another plugin to speed up their cutting 40 to 60 % here
in this thread I mention this and provide some info.

Will try it too, thank you for letting me kow, I haven''t browsed the plugins page in a while, nor the forums, but I always know you guys helped me EVERYTIME, I recommand CamBam to anyone I talk, even if NOW I mostly work in fusion360 drawing/3d modeling/programing my Tormach mill, my colleague works daily in CamBam as he mostly works on the CNC router.
When I started working with cambam I made lot's of styles, for most materials we mill and after I showed him the main options of CamBam it was so easy for him to program the router and mill the parts, cambam rocks!! I love how easy and quick you can do the job with it. BTW.. the freaking Fusion360, even now, after 2 years since I started to work with it doesn't support import of text from DXF files, it's so stupid, such an advanced program doesn't have such a basic feature!! And the solution is good old cambam :)) Open the dxf in cambam , convert text to poly, and than export again the dxf

Sibianul are you using this grade of brass as it machines very nicely.

For some of the gummy Aluminium and Brass I use a HSS two flute slot drill and for a lubricant use either Kerosene or Diesel. Both are a bit smelly but give a very nice finish WD40 is also good but I don't always have it on hand.

That's a very nice Router by the way.

I sincerely don't know the alloy of the brass, but it's not gummy at all, not like aluminium, but it's harder, to hard for me to try making slots, or deeper slots. And now most of the aluminium part I try to mill them on the Tormach Mill, where I use  coolant, aluminum is milled so easily on the tormach, but I don;t have very often jobs in aluminum, most of the parts I make on the Tormach are steel parts.

BTW . I plan to build a smaller mill, about 160x120mm travel, only to mill the brass stamps, hope in the next few months will have enough free time for it :) I have a spare 2.2kw chinese water cooled spindle and inverter, it's a little big for such a small machine, but I think I will use that.

I had a look at the file and generated the toolpaths, I received a lot of Troc mop errors.
All the errors are generated by the first trocopocket because it very often fails to jump from an "island" to another, but some times its able to mill all islands, very rarely, but it happen. I don't know why, I just know it doesn't work ok when it can't mill the entire surface because it has an area too tight to continue with semicircles toolpaths, instead of making a retract and than a spiral plugne in the next island, it shows that warning.
In the picture bellow I marked the areas where trocopocket wasn't able to generate toolpaths, even if the end mill was small enough, it just couldn't generate an retract and another spiral plunge in that area. I'm used to it, and my quick fix is this:
1. I copy paste the initial operation and add manually a start point in one of the unmachined areas.
2. If there are multiple areas, I duplicate that MOP multiple times and chose a different start point for each one, as you can see in the attached .cb file.  

What I did was generate new mops and used the collision detector.
To save time on my old computer I changed the target depth to 0.5 mm (simulating was too slow).
At this depth, using an endmll or vee bit doesn't make too much difference.

I've re-posted the CB file with my adjustments for the first Key Fob.
It looks Ok in the simulation.
I used 2 mm,1 mm and 0.5 mm cutters here and tomorrow night I'll look at the vee cutters.

I usually mill the brass stamps to a depth of 3mm or 4mm, I love trocopocket MOP at this depth in brass, with an 3mm endmill, and I don't think a simple pocket would be better (can you mill at -3mm with a 3mm endmill, without breaking it?), what I don't like at all on normal pocket MOP is:
1.  when it begins, after it plunges to target depth it mills with an 100% tool engagement, and I wasn't too lucky when tried small 3mm endmills in brass or aluminum, maybe you guys know other tricks, but I failed multiple times, to not brake the endmill I had to do multiple passes with a small DOC, and this leads to the second reason I prefer TROCOPOCKET instead of NORMAL POCKET. If I chose Lead in spiral I can limit this 100% engagement of the tool.
2. when milling brass and aluminium only (in policarbonate, mdf, textolit - fiberglass I always use normal pocket) instead of using small DOC, and wear only the 0.5 - 1mm of the tool, I prefer TrocoPocket MOP and plunge to target depth directly, in brass with a 3.175mm endmill I can easily mill directly at -4mm, in 7075 aluminium I remember once I milled with a 4mm 3flute end mill,  directly at -10mm, trocopocket rocks ! :D

The Collision Detector wasn't really made for vee cutters, however if you are really determined to
to the job, then you could generate the tool paths with the CC and offset them per the sine rule.
In most cases there isn't any problem with the collision detector and vee cutters because I always use the mighty SIDE PROFILE option (I LOVE IT !!! :D ) Now I noticed one small detail, in the open lock polyline, because some lines generated fragmented, when it does the SLOPE PROFILE, the V-bit will mill an area that shouldn't be milled

I attached a CB file with the way I would do it and I mention a few things I think might be improved :)

1. The unmachined generated line, I  think it's to exact in length, I think it should overpass the machined area a little to have a cleaner surface, isn't it ?
To fix this, I will try to write a bigger diameter for the initial tool, bigger than it actually is. For example, if I mill with 3mm EM and clean up corners with 2mm , I write 4 on the TEST THIS CUTTER field, and 2mm on the  Clean up MOP. This way, the generated line is longer.

2. Many lines need to be inverted, on this key model it's not a big deal, but on more complicated models it's very easy to miss an line that needs to be reversed

3. In my case when I tried to generate Unmachined areas from 2mm to 0.5mm, for the cars open trunk, it didn't generated any line.
On the Brass emboss stamps, I use
  • 3.175mm flat end mill to do the trocopocket
  • than a 2.3mm or a 2mm flat endmill to make all the contours again
  • than I start with V type end mills, first 1mm tip or 0.5mm tip, and the finish MOP with a 0.2mm tip, 15 to 30 degree angle

Thank you Dave for all the detailed replies, I now know how to use the plugin :D It's only the bottom slider that doesn't do what I expected, I hoped that could extend the generated lines, but somehow it seems it makes the lines shorter. Anyway, I will try to use it  on my next stamps I will need to make next week.

I also want to build a smaller machine especially for leather stamps, a smaller router, but sturdy :) 

Hello Dave, sorry for the delayed response but I've been so busy, actually I'm still in the workshop now, saturday night at 8pm...

I really appreciate your responses, and will check the plugin and your examples tomorrow, when I won't be in my workshop :)

I was so busy that I left the new BIG CNC router we purchased, in the box for more than a week, and today my brother decided to unpack it as he seen I still don't have time to do it myself, a few days ago I told him I was extremely curious if the metal parts rusted while it was on the ship from china to Romania. It seems Andy from union-cnc did a good job protecting all the untreated metal parts, as I asked him before shipping :) I will post some new messages regarding the new router, as I don't know exactly what software to use to make the CAM for the 4th axis.

Thank you Dave, I don't know yet if in my case it's a little more complicated as I use mostly 30 degree V-bits. First I make a roughing pass with an flat 3.175mm End mill, and than a second roughing pass with a 30 degree V-bit, with a 0.5mm tip. Than the finish pass with a 30deg - 0.2mm tip V-bit.

I attached the cb file with my current operations.

Thank you , I will check the documentation and let you know if it does the jo, so far I tried it without reading the documentation and haven't had any luck, I'm sure I NEED TO READ THE PDF to understant how the script works.

PS. The reply notification was marked as spam, if the admin is around maybe he can check those headers, I can provide complete headers if it's needed

Code: [Select]
Content-Type: multipart/alternative; boundary="SMF-e2a7a6666cf62851ce97405200dfcf3a"
Content-Transfer-Encoding: 7bit
X-OriginalArrivalTime: 30 Jan 2020 18:25:17.0516 (UTC) FILETIME=[9F51A0C0:01D5D79A]
X-Spam-Status: Yes, score=5.5
X-Spam-Score: 55
X-Spam-Bar: +++++
X-Spam-Report: Spam detection software, running on the system "",
    has identified this incoming email as possible spam. The original
    message has been attached to this so you can view it or label
    similar future email. If you have any questions, see
    root\@localhost for details.
    Content preview: A reply has been posted to a topic you are watching by EddyCurrent.
    View the reply at:;topicseen#new
    Unsubscribe to this topic by clicking here:;topic=6857.0
    Content analysis details: (5.5 points, 5.0 required)
    pts rule name description
    ---- ---------------------- --------------------------------------------------
    -1.9 BAYES_00 BODY: Bayes spam probability is 0 to 1%
    [score: 0.0000]
    0.8 KAM_COUK Scoring emails higher due to poor registry
    1.5 SPF_HELO_SOFTFAIL SPF: HELO does not match SPF record (softfail)
    1.5 SPF_SOFTFAIL SPF: sender does not match SPF record (softfail)
    1.6 DATE_IN_PAST_03_06 Date: is 3 to 6 hours before Received: date
    2.0 RDNS_NONE Delivered to internal network by a host with no rDNS
X-Spam-Flag: YES
Subject: ***SPAM*** Topic reply: Rest machining - for me, the "only" missing feature in CamBam!

Haven't posted in a while on this forum, but I still use CamBam daily, as before, for 2D jobs on my CNC router. Fusion360 is the same used daily for my 3D metal parts I make on the mill.

I want to ask again if there is anyone interested to tell me/us the fee needed to build a plugin, to have this REST MACHINING feature for basic OPS like profiles, pockets.

It will be an huge improvement in milling time, for example on those brass stamps, where I mill with vbits with 0.2mm and 0.5mm tip, most of the cuts need to be made only on internal corners, and all the other flat, lightly curved toolpaths just mill air :(

I will try again the v-carve plugin, to see if I can use that, but I remember that years ago when I tried it , it did some overcuts on the corners, and on brass stamps with very small details it didn't work too good.

Hello guys, I haven't posted for a while, but today I decided to ask you guys something, as is the second time in a few years, when something is wrong with my UPS, and the PC turned off when the power was lost for a second or less, I will change the UPS anyway, but I never never used the .b1, .b2 or .b3 files that are generated when I save a cb file, I always delete them.

Isn't a better idea to have an option to autosave the file each x minutes ? I think this would be much more useful than the other backup feature that is already implemented (creating another file only when I manually save my project). I just lost a file I worked for more than an hour :(

Thank you.

Maybe I didn't get all the details but it seems this part is perfectly doable in 2.5D.

I still don't know exactly what 2.5D means, if it regarding the ability to move 3 axes in the same time or the fact that the milling can be made only top - bottom, and not under (like on 5 axis machines where it's needed to rotate the part, to reach some areas that can be reached from the top side)

Here's a video while I milled that line, it's just a simple engrave operation made in CamBam, all 3 axes move in the same time. But my problem was not the CAM part, I knew from the begining how I would mill that, my only issue was drawing (bending) those lines.

David, that part I made yesterday is used to perfectly centering and glue together the 2 leather pieces. Usually they tell me to make flat blocks, for glueing together the 2 parts, but in this specific case, after they glued the parts together on a flat surface, they had some problems with the inner leather part when bending it like in my pictures (it curled I think), that piece of leather will be a bags handle, and the final shape will be a curved one, like the big MDF block I made.

My clients are usually big brands, that charge hundreds or more than 1k Euro for a single leather bag, so they need all kind of "devices" in the production process to perfectly make each part of the bags, avoiding to rely only on the worker skill, with parts like the one I made yesterday, all the leather pieces are perfectly aligned, in the next steps of the production process, the result of perfectly aligning the 2 leather parts will be noticed, because they cut those lether parts again, and they sew them, if the inner part will be just 1mm glued more to a side, that results in noticeable defect On some parts they sew the leather on automatic machines, that are programmed (like CNCs) to make an exact number of punches on a specific distance, not having the parts aligned perfectly is even more noticeable in those cases.

Bubba, I appreciate everyone's help, even the reply Armando made, but I already tried that projection function as you can see in the picture I attached in my first post. Resizing the polyline to be bended I don't think it's an option, I don't know what formulas I can use to resize that perfectly, also as you seen it's not just a radius but half the polyline is bended on a radius and another half is bended at an angled surface.
The resized polyline that Armando posted, resulted in a very different shape, it was clearly that I could not fit my leather parts in the resulted projected shape. The difference are better noticed in the bellow screenshot.

I just finished milling the part, it came out perfectly, I'm very happy with the result.

To be able to mill on the variable depth, I used the engrave function, and to have the channel width as in the initial drawing (one 3mm and one 4.2mm) I used different end mills for the engrave operation, for the 3mm width of channel, I used the 6mm end mill, and for 4.2mm channel, I used an 8mm end mill, the 0.2mm difference is not an issue on this part.

Thank you David for your help!

Pages: [1] 2 3 ... 19